GTA
All Springer/NP/PCP Air Gun Discussion General => Machine Shop Talk & AG Parts Machining => Engineering- Research & Development => Topic started by: WobblyHand on May 02, 2023, 10:47:49 PM
-
The recent thread on a ruptured pressure vessel, reminded me that HPA can be dangerous. I was wondering if there were tools that could help us analyze things like this, and could be used by folks that hadn't done this kind of work for a living. I'm thinking in terms of people that want to make or machine items for airguns.
Many CAD packages have some level of finite element analysis tools. Ones that have these FEA packages include Fusion360, SolidWorks, FreeCAD, and I'm sure others. The question I had was how hard is it to actually do this analysis. Turns out, it's not too hard, at least in FreeCAD to do FEA. FreeCAD being non-commercial, isn't quite as slick as the other tools, but, it seems to work ok, once you figure out a few quirks. Now I am not a mechanical engineer, nor have I done this professionally, but I have had exposure to FEA for solving electromagnetic problems.
The basic steps are as follows
- Create a model of the structure under test
- Add any fixed constraints
- Apply pressure constraints
- Apply the material
- Mesh the model
- Set up the Solver and run the Solver
- View the results
Here's a simplified model, hey we have to start somewhere. It's 38.5mm OD with 3mm walls. It has a horrible sharp inside corner, which we know is not good for a pressure vessel. Lets say it is made of 6061-T6 and we charge it to 300 MPa. To the right side of the line is pressurized. Then we put some constraints. We mesh the model. At least in FreeCAD, it's a good idea to constrain the maximum element size. Since this model is roughly 150 mm long, I chose a max element size of 1.5 mm. The meshing takes a little bit. Then one runs the solver. At least on my PC, it uses all the CPU cores for solving. On an i7 it took 30 seconds.
We can show various results including von Mises Stress, Max Shear Stress, and displacement.
What I am trying to learn still is where and how to constrain the model. This took me a couple of days to figure out so far. Have a lot more to learn. I can post the model if anyone is interested. My original model had the vessel threads in it, but I stripped them out, since they were not in the pressure region.
-
As you practice a bit, it gets a little easier. (Instead of being clueless, I have progressed to slightly befuddled ;) )Here's the interior view of a pressure cylinder made of 7075-T6 running at 105 MPa, 3.5 x its working load. You can see the stress induced by the sharp interior edge. Had to play with some of the defaults in FreeCAD to get this to render correctly. The default is no anti-aliasing, which is a poor choice. I set the anti-aliasing setting to MSAA-4x, and the formerly gray interior now seems to be rendered better. In a while, I will radius that inside corner, because we all know that is the right way to do it.
Been interesting doing this. Makes me leery of using aluminum pressure cylinders... Wonder what titanium would be like? (A devil to machine!)
-
I’ve no input here but enjoy your explanations. Very interesting subject for sure. Keep us updated.
Dave
-
Interesting thread for the software your using.
Can't say that I really care for the programs being used by Marco or Ed.
And I have to wonder IF both are using the exact same 3D mesh and how accurate the mesh is to the final produced part.
-
Interesting thread for the software your using.
Can't say that I really care for the programs being used by Marco or Ed.
And I have to wonder IF both are using the exact same 3D mesh and how accurate the mesh is to the final produced part.
I think Marko uses Fusion360, not sure about Ed. Unlikely they are using the same mesh. Ed, unlike Marko has the original drawings. Marko is measuring "used equipment". Not sure if that is good or bad. Perhaps you could say Marko is using "as built".
The meshing on FreeCAD is sort of ok. I simply controlled the maximum cell size and let it figure it out from there. Fusion360 and all the other packages may have smarter routines. All meshers will fill the model. There will not be any unmeshed areas - that would trigger a meshing error. It's possible to zoom in on the mesh and verify full coverage.
I'm so far from being expert at this... But it has been interesting working on FEA. I'm now trying a cylinder with a rounded bottom. Having trouble with FreeCAD meshing and constraining, due to me not understanding some key point. I'll figure it out eventually.
-
Was having a little trouble with meshing the cylinder, and found I had an old version of the mesher. Updated the mesher and it easily did the cylinder with rounded inside corners. The solver had fewer issues with the mesh and was quicker as well, so that's a win win. The stresses are a bit more spread out over a larger area, primarily over the fillet area. Material: 7075-T6, 3mm wall thickness, 105 MPa. (3.5X operating pressure) Peak von Mises Stress is still high at 639 MPa. I used a 1.200 mm largest element size for the mesh. Curiously a 1.250 mm mesh had errors in it. Running at a 1mm mesh gave the same peak stress, to within 0.1%, but took more than twice as long to run. Not going to lie, the application tends to favor server grade computation and memory sizes. Peak memory consumption was around 28 GB, for the 1mm mesh, so it was getting close to the limit on my laptop with only 32 GB RAM. But running at finer and finer mesh only seems to refine the answer by a minuscule amount - and is usually only used as a sanity check. Most of the time a coarser mesh is perfectly acceptable. Or simplifying the model. I put in threads in the model, which strictly speaking, is not required, since they are out of the HPA zone. Lots of ways to make the model fit, if required.
-
Turns out the meshing was a little coarse in the example above. Went to a finer mesh, which does stress memory constraints, on my 32GB system. Went to a 0.990mm mesh, which guaranteed there were at least 3 elements in the thickness of the pressure tube. Probably should make the cell smaller, but that's pushing it on my laptop. But now we can see the stresses in the cylinder, which seem to make some sense. In the curved region (5mm radius) the stresses are moderate. The peak stresses are on the inner surface where the HPA resides. There's clearly an art to this - as well as the science. First picture is with 50% transparency, so you can see through the part. Second picture is 0% transparent, but the cylinder has been cut in half lengthwise so you can see inside. The second picture shows the maximum stress is on the inner surface.
-
At 105 MPa, (3.5x operating pressure) the von Mises stress (638 MPa) is well over the typical yield strength of 7075-T6 (503 MPa). The von Mises stress is also greater than the ultimate strength of 572 MPa. Doesn't seem like a safe area to operate...
At 90 MPa (3x operating pressure) the von Mises stress is 547 MPa, which is still higher than the typical yield strength of 7075-T6 and somewhat close to the typical ultimate strength of 572 MPa. Still not quite a happy place to be, if I am understanding correctly. I think this means there will be permanent deformation of the cylinder at 90 MPa, but I'm just a dabbler at this.
At 75 MPa (2.5x operating pressure) the maximum von Mises stress is 456 MPa, which is under both the typical yield strength and the ultimate strength. So not likely to have an issue, he naively thinks. So roughly speaking, this design has about a 2.5x safety factor.
Please don't design to this and think it is safe - this is merely an engineering exercise - make sure you verify any of your designs to make sure they are safe! I am not a professional mechanical engineer, I do not have access to the minimum values of the material properties, nor have I learned all the rules of thumb, so take all my comments above with a grain of salt. Merely the ramblings of an amateur.
-
How accurate is the scale of your Model? I mean is it to scale of the Real World part?
Not trying to start a problem just want to understand.
-
How accurate is the scale of your Model? I mean is it to scale of the Real World part?
Not trying to start a problem just want to understand.
Don't honestly know Jeff. I looked at the photos in the epic thread, and estimated values based on a couple of measured values that Marko showed, and the proportions relative to those measurements. So it's a WAG, but not too far off. The model above I used a 5mm radius on the end, rather than a sharp inside corner. Within the guide lines Marko mentioned for a 3mm wall. As far as I know, Marko didn't publish that many dimensions, perhaps not to publicly show the dimensions (as a courtesy?). If I had better dimensions, of course the model and results would be better.
I simulated 7075-T6 above. That is what I am guessing that has 2.5x safety factor. Not 2024 (D16T) which is the material for the actual tube.
2024-T4 is not as strong... Yield strength of 2024-T4 is 324 MPa, but 7075-T6 is 503 MPa. Ultimate strength 2024-T4 469 MPa vs 7075-T6 572 MPa. https://asm.matweb.com/search/SpecificMaterial.asp?bassnum=MA2024T4
https://asm.matweb.com/search/SpecificMaterial.asp?bassnum=MA7075T6
I'm not a professional ME. Just dabbling in this, because it really caught my attention.
BTW, I agree, Ansys is a professional grade simulator. We used HFSS (an Ansys product) for RF simulations for quite a while. We found it didn't scale well for the really huge problems we wanted to simulate for millimeter wave radar, so we transitioned to a different technology using GPU's. This was because the new technology could use/exploit massive parallelism and use GPU's for computation. We achieved 30-100x faster solutions than using HFSS, which didn't exploit parallelism. This meant simulations that took days the old way now took under an hour. The new method called Finite Difference Time Domain, allowed us to see electromagnetic waves as they were propagating and how they interacted with the structure. HFSS in contrast was a steady state solution. We were able to massively increase our understanding and throughput using the new system. I don't know if HFSS has been updated to use GPU's. It was a rough transition at our company, with the HFSS guys having to learn new ways... We also had to install huge fast disk farms - if I recall correctly, we had 1 Exabyte capacity. It was a major problem just shuttling data around, due to the puny 10GbE networks we had, because moving 10TB files took a significant amount of time! These are typical problems with high performance computing - there are bottlenecks in the most unforeseen places.
Anyways, this is a mechanical FEA thread, not electromagnetic one, sorry for the digression.
-
I totally understand. I think that's where people went all crazy on me. I believe to fully understand a problem people need to share data.
It's called Peer Review. I bet you'd LOVE my friends HOME system! That thing is CRAZY beyound belief!
-
I totally understand. I think that's where people went all crazy on me. I believe to fully understand a problem people need to share data.
It's called Peer Review. I bet you'd LOVE my friends HOME system! That thing is CRAZY beyound belief!
I agree. Peer review is indeed a good thing. WAGging the dimensions, is not so good, but all I have.
Sound like a very cool computer setup. Would be neat to see. Of course, I'd want to see what it could do! Always testing the limits!
I'm going to do a 2024 simulation using the identical mesh, at 2.5x rated pressure for giggles. I'm sure I will have to back off the pressure, at least not to have it yield on me. Unfortunately, my SW won't tell me something is about to explode, but it will give me the stresses, and I can compare them to the published material properties. Best I can do.
-
He's stepping up to an Epyc before long. 128 core 256 thread, with 256 GB of ECC RAM (4TB max)!
-
Looks like the same design in 2024, has a safety factor (no yield, well under ultimate tensile stress) of a smidge under 2:1, best I can tell. This is assuming 2024T4.
I get von Mises stress = 365 MPa. This compares to UTS (ultimate tensile stress) 427, so we are good there, and yield stress of 305 min, 324 MPa typical. The simulation shows the tube grows by 91um. I don't know how much of that is permanent - that's beyond my pay grade. This is a static simulation (linear). Perhaps the answer is different using a non-linear sim.
7075T6 is definitely superior, allowing a 2.5x no yield margin.
Without radiusing the corner, 2024 doesn't seem like a very good choice, at least to my inexpert opinion. The radiused corner doesn't even make 2x yield safety factor. Seems like trouble waiting to happen. But that's only my inexpert opinion, based on swag numbers from crooked pictures...
-
I have to wonder something.
That area is supported somewhat.
So how likely would that support hold that area from catastrophic failure as seen in the pictures?
That may be why there was no sever injuries.
-
I have to wonder something.
That area is supported somewhat.
So how likely would that support hold that area from catastrophic failure as seen in the pictures?
That may be why there was no sever injuries.
Have a picture of that? Not really that familiar with how that AG is setup.
I did model this once, but it was a pain in the neck. I had to fuse two pieces together and it was tough to edit afterwards. If I had known it was tough to edit, I would have modeled it differently. The pitfalls of modeling - there are many ways that work, but some are way better to use!
-
He's stepping up to an Epyc before long. 128 core 256 thread, with 256 GB of ECC RAM (4TB max)!
What does he do with the old computers?
-
Here's a quick image.
The Red arrow is where the failure was.
The Blue arrow is the brace.
So I suspect a sideways rupture after the end failed near the red arrow area.
Being covered by the neoprene? That burst of air is what shredded it.
-
He's stepping up to an Epyc before long. 128 core 256 thread, with 256 GB of ECC RAM (4TB max)!
What does he do with the old computers?
He runs them as backup for now. He is a Operating Systems Programmer.
Just his network in his home is near to a PetaByte of data storage!
His home Network operates at 20 Gigabyte times 2!
All fiber Optics.
-
Here's a quick image.
The Red arrow is where the failure was.
The Blue arrow is the brace.
So I suspect a sideways rupture after the end failed near the red arrow area.
Being covered by the neoprene? That burst of air is what shredded it.
Thanks for that. I didn't model that area. Looking at the dimensions, it looked beefy. And it is pretty clear the fracture was not in that area. I modeled the versions with a fixed constraint pushing against the bottom of the cylinder. I also have a high uncertainty of the dimensions there. Apparently there is a threaded hole there, and possibly a narrow diameter hole into the cylinder? Happen to know the diameter of the threaded hole? (M6? M8?) The tiny through hole diameter, if it indeed goes through? To be honest, those details seem pretty far removed from the explosion zone. The fracture looks like it is at the base of the main diameter, which is roughly 5mm away from the rest of the area. Hard to say what the actual sequence of events was during the rupture - outside of my experience.
-
That is why I asked BOTH Ed and Marco for thier models and information.
Peer Review is important!
You could easily post your work and have others just accept it as TRUTH and FACT.
You are seeing the limits of your home system. What kind of systems do Ed and Marco run?
Another part of the question on results.
-
@Privateer "So how likely would that support hold that area from catastrophic failure as seen in the pictures?"
I don't think it would do much at all. It doesn't look like a strong junction, but I'm no expert. I don't even play one on TV. Shoot, I couldn't even pass for an expert on AGN :-X
It would have been a lot better for everyone to have posted a couple of drawings, like a section drawing pdf, that folks could model. However, I do understand that most manufacturers do not do this, American one's included. And I do understand Marko not posting either, since he may not have wanted to violate this "standard". I suppose I could request a section drawing from Marko, maybe he would supply one to me. Honestly, I don't know why he'd bother with me, I'm just a nobody on this forum, with a scanty number of posts, or accomplishments.
As for others accepting anything that I say, well, you have witnessed the pecking order here and at AGN. I'm so low on the totem pole I have no street cred. I'm only doing this investigation, because it made me extremely curious what happened. It would be good to know, and to share the information, if anyone was open to looking at it. I'm sure that an experienced ME would get to the bottom of the analysis a whole heck of a lot faster than myself, and would have a significantly higher chance of being correct. My only advantage is that I am unencumbered by experience, but that could easily lead me astray.
-
You are seeing the limits of your home system. What kind of systems do Ed and Marco run?
Of course. Big sims eat up memory. I could remove the threads and chop off that part of the model, and then I could exploit symmetry if I was super serious about all this, that's what the HFSS guys had to do all the time, because their servers were never big enough. Me, I'm just running Linus on a laptop with only 32GB RAM. My laptop has some issues, so I'm not anxious to buy more RAM for it, even if I could install more. My next machine will have more RAM, might get a desk machine for that. The computer won't be as capable as your neighbor's, I'm retired so no big bucks for that stuff. Might even build one up, like I used to do, but the economics are not that favorable these days.
Really don't know what the other guys have. I vaguely recall Marko mentioning running in the cloud. I don't know how to do this, except perhaps as an EC2 instance, and at the moment, I don't know how to do that. Then there is always the problem of transporting the data back...
-
I could double my RAM to 64GB. That would max out my laptop. Found some DDR4 SO-DIMM 3200 MHz RAM for around $120 for 2 - 32GB sticks. Not sure if I will go for it, maybe if I can shop around and find a better price.
What I can't believe are all the alleged workstation grade PC's that are being sold with only 16GB, like that's pitiful for a workstation...
-
Jeff, if your friend wants to help us out, have him run a few generic examples of a flat bottomed cylinder with different bottom thicknesses and radii between the cylindrical wall and the bottom.... For a given pressure and material, the thickness/diameter ratio is a constant for equal safety margin.... Also, the required wall thickness (for a given diameter) is basically proportional to the pressure.... So, draw up a generic tube, for example a 1" ID with a 0.125" wall, (so an OD of 1.125") made from 2024-T3.... The ID to wall thickness ratio is 8:1, using the OD it is 10:1.... My calculator says that at 300 bar (4350 psi), the safety margin to yield is 2.5:1, and to burst is 3.5:1, which I would be fine using (and in fact have).... Determine the hoop stress at 300 bar (4350 psi).... Using 50 Ksi Yield and 70 Ksi Tensile for the 2024-T3, I get 19,817 psi using Lloyd's calculator, based on thick-walled tubes (our reservoirs are not thin walled, that is for a wall thickness of less than 5% of the ID)....
Have him add a flat bottom, same material, starting at, say, 0.250" wall (twice the cylinder wall), and keep increasing the thickness (or decreasing it) until the stress in the center of the bottom is (just) less than the hoop stress.... Don't worry about the high stress in the corner where they meet for now.... Once he has determined the required thickness in the middle of the bottom, have him add a radius to the inside corner of 0.125" (equal to the wall thickness), and keep increasing (or decreasing) that radius until the stress falls below the hoop stress in the cylinder walls.... Now you have a safe configuration for a reservoir of those dimensions, right?
A few other runs, changing the pressure, material strength, and dimensions, should give us what we need to design a safe flat-bottomed reservoir.... At least we would know if there is a simple answer, or if a change to the T/D ratio requires a change to the thickness of the bottom and the radius (when expressed in wall thicknesses)....
Bob
-
There is something remarkable in Ed's drawings that real professional should notice immediately. Something is just the same way in every picture that cannot be true and something is missing. I don't tell anything more now, let our "professional" tell us from these tips...
-
That is why I asked BOTH Ed and Marco for thier models and information.
Peer Review is important!
You could easily post your work and have others just accept it as TRUTH and FACT.
You are seeing the limits of your home system. What kind of systems do Ed and Marco run?
Another part of the question on results.
Where did you directly ask for the model? Have not seen a post about you directly asking me could you have the model?
Fusion uses cloud computing for simulations, data is sent out and results recived after the simulation completed. Have simulated stuff on site that took hours and over there it takes 10-15 minutes, so I don't think Autodesk are running an old hand me down for their servers.
Marko
-
That is why I asked BOTH Ed and Marco for thier models and information.
Peer Review is important!
You could easily post your work and have others just accept it as TRUTH and FACT.
You are seeing the limits of your home system. What kind of systems do Ed and Marco run?
Another part of the question on results.
Where did you directly ask for the model? Have not seen a post about you directly asking me could you have the model?
Fusion uses cloud computing for simulations, data is sent out and results recived after the simulation completed. Have simulated stuff on site that took hours and over there it takes 10-15 minutes, so I don't think Autodesk are running an old hand me down for their servers.
Marko
Marko, can you provide a dimensioned section view drawing of the tube? My simple FEA analysis was based on some assumptions and extrapolation from your pictures. Would be good to have more validated dimensions. A simple section view PDF would suffice, as the piece has symmetry (ignoring threads). I don't have access to huge computers, but there's still a lot that can be learned on a desktop machine.
The point of my thread is we can do some level of FEA on desktop class machines, if we are knowledgeable. If we can pass that knowledge along, the whole airgun community benefits. We can also identify designs or concepts that need improvement.
Like you, my sims show stresses above yield point of 2024 at least for some configurations. This thread is not to criticize anyone, but to learn and highlight any issues.
Thanks,
Bruce
-
Now lets stop this conversation about home computers and supercomputers. Just press ctrl+alt+del, choose task manager, then performance and see how many threads you have active.
Well now, how can your computer survive to run windows?
Also, we have here just a simple problem with a tiny simple tube, not a complete space shuttle. Before computers this was made by pen and paper.
-
Now lets stop this conversation about home computers and supercomputers. Just press ctrl+alt+del, choose task manager, then performance and see how many threads you have active.
Well now, how can your computer survive to run windows?
Also, we have here just a simple problem with a tiny simple tube, not a complete space shuttle. Before computers this was made by pen and paper.
Let's continue to be pleasant and conversational in this thread. A discussion of colleagues, not adversaries.
My point is a home computer can do some level of FEA. This is a simple design, I agree. Pen and paper are very useful as well, and I use them often :).
FEA can highlight problem areas, that may not be obvious when using pen and pencil. FEA shows where the stresses are physically. However, numerical simulation doesn't give us general guidelines, it only shows us the solution to the exact problem we simulated. If we simulate enough, then perhaps we can make some generalizations. FEA can require a lot of memory, especially at fine meshes, but exploiting symmetry can reduce the memory footprint if necessary.
Would be nice to have a cross section drawing, if it could be made available. A PDF would be great. Thanks, Bruce.
-
That is why I asked BOTH Ed and Marco for thier models and information.
Peer Review is important!
You could easily post your work and have others just accept it as TRUTH and FACT.
You are seeing the limits of your home system. What kind of systems do Ed and Marco run?
Another part of the question on results.
Where did you directly ask for the model? Have not seen a post about you directly asking me could you have the model?
Here Ya go!
https://www.airgunnation.com/threads/leshiy-2-explodes.1284424/page-27#post-1486138 (https://www.airgunnation.com/threads/leshiy-2-explodes.1284424/page-27#post-1486138)
I did ASK for 3D meshes and information from both parties!
Just because a 3rd party questions things does not mean that 3rd party is an advisary to the 2 other parties.
-
That is why I asked BOTH Ed and Marco for thier models and information.
Peer Review is important!
You could easily post your work and have others just accept it as TRUTH and FACT.
You are seeing the limits of your home system. What kind of systems do Ed and Marco run?
Another part of the question on results.
Where did you directly ask for the model? Have not seen a post about you directly asking me could you have the model?
Here Ya go!
https://www.airgunnation.com/threads/leshiy-2-explodes.1284424/page-27#post-1486138 (https://www.airgunnation.com/threads/leshiy-2-explodes.1284424/page-27#post-1486138)
Honestly, (in my opinion) just the measured dimensions of the tube cross section(s) are fine. The issue with exporting the mesh is compatibility and possibly size. Anyone who has the dimensions can mesh the model to the level they need. Also it is a lot easier to make changes on a model than a mesh. The model is simple enough a couple of drawings would be sufficient to recreate it in the CAD system of your choice.
-
That is why I asked BOTH Ed and Marco for thier models and information.
Peer Review is important!
You could easily post your work and have others just accept it as TRUTH and FACT.
You are seeing the limits of your home system. What kind of systems do Ed and Marco run?
Another part of the question on results.
Where did you directly ask for the model? Have not seen a post about you directly asking me could you have the model?
Here Ya go!
https://www.airgunnation.com/threads/leshiy-2-explodes.1284424/page-27#post-1486138 (https://www.airgunnation.com/threads/leshiy-2-explodes.1284424/page-27#post-1486138)
I did ASK for 3D meshes and information from both parties!
Just because a 3rd party questions things does not mean that 3rd party is an advisary to the 2 other parties.
Ok I have missed that.
-
Can We just be friends now then?
I named one of my Rescuse kitty's Kohtalo!
And believe it or not? I have a friend named Teemu in Findland.
-
The cylinder details matter. As mentioned in this thread, and elsewhere, sharp inside corners are stress risers.
Here's a cut away view of the stress riser, which has a maximum value of 355 MPa, but the yield of 2024T6 is about 305 MPa. This is with the cylinder charged to 30 MPa, which is the rated pressure. You can see the red and yellow ring, right in the sharp corner. The safety factor to yield is less than 1. For my model, which only has estimated dimensions, I get a safety factor of about 0.86. Obviously this isn't good. Will it blow immediately, not likely. After a lot of cycling this area will certainly be weakened. It is interesting that one of the fragments showed a fracture in this area.
-
I have received some better measurements for the air cylinder, courtesy of Marko. Thanks. Will modify my model to make it the same as the provided details. The cylinder walls are slightly thicker than I had initially estimated. Will update this thread when I have some results. I'll put in a typical insert cutting tip radius for the inside corner, about 0.4 mm, which seems to be a standard size. (For a CCGT type insert.)
-
Such a simple thing to avoid, at the penalty of losing just a bit of volume.... ::)
Wobbly.... Once you have the correct dimensions, I am looking forward to seeing an FEA run at 100 MPa, the pressure a 30 MPa cylinder should be designed for!.... If the cylinder walls pass the hoop strength required at that pressure, and you feel like a bit more work, try an end wall twice the tube thickness, with simple square outside corners, and then do a run with an internal radius equal to the tube wall thickness.... PLEASE!!!!
(https://hosting.photobucket.com/images/oo221/rsterne/Test_s6aqAH7NEZzhSSU2BfMh1Z.jpg) (https://hosting.photobucket.com/images/oo221/rsterne/Test_s6aqAH7NEZzhSSU2BfMh1Z.jpg)
The above sketch is to give you the idea of what I would like to see tested.... THANKS!!!!
Bob
-
Such a simple thing to avoid, at the penalty of losing just a bit of volume.... ::)
Wobbly.... Once you have the correct dimensions, I am looking forward to seeing an FEA run at 100 MPa, the pressure a 30 MPa cylinder should be designed for!.... If the cylinder walls pass the hoop strength required at that pressure, and you feel like a bit more work, try an end wall twice the tube thickness, with simple square outside corners, and then do a run with an internal radius equal to the tube wall thickness.... PLEASE!!!!
(https://hosting.photobucket.com/images/oo221/rsterne/Test_s6aqAH7NEZzhSSU2BfMh1Z.jpg) (https://hosting.photobucket.com/images/oo221/rsterne/Test_s6aqAH7NEZzhSSU2BfMh1Z.jpg)
The above sketch is to give you the idea of what I would like to see tested.... THANKS!!!!
Bob
Yes, that is exactly the idea of what I want to do! I have the model done, with a radius of 0.4mm for the inside corner. My CCGT boring bar inserts have that tip radius. I will do that first. Then increase the radius to about 3.3mm or so (tube thickness). For a little more fun, I will increase it to 2x the tube thickness, which should be more than enough.
Meshing still seems to be an art. Sometimes it works for me, and other times not. Think there's either a problem with how I constructed the model (don't know why, but) or the SW. I will get the meshing sorted out eventually. Getting a few cryptic messages, so FreeCAD isn't happy about something. I converted the threads to pseudo-threads, so the model would be symmetric, around the cylinder axis, which shouldn't affect the results, since the threads are in a low pressure zone. If I need to, I could simulate 1/2 the cylinder, or 1/4 of it, to reduce the problem size. I would only do that if I ran into memory problems. The rest of the model is based on Marko's measurements. Here's a transparent view of what I have so far. I don't know the angle of the chamfer between the HPA are and the low pressure. I modeled it as a 45 degree chamfer, to give it a value. Not hard to change, just don't know a reasonable value for it - so 45 degrees it is.
Just for clarification, do you want 3.5x factor? 105 MPa?
-
I'd still like to have your actual 3D Model. (And Ed's and Marko's)
I've been a 3D Modeler since around 2006 or so. Many of my models were used in Games over the years.
-
Well then Jeff, how are you not seeing what is wrong in Ed's pictures? I will show you.
These pictures are exactly from the same model, same mesh, same study. Nonlinear 65MPa pressure. Ed's way of presentation first:
(https://img.aijaa.com/b/00249/15149902.jpg)
Then how it comes without modification:
(https://img.aijaa.com/b/00458/15149905.jpg)
Do they look different? Why they do look different? Why didn't you see it?
Presentation of the same result makes it. Why there is a full scale of stress ditribution between exactly 0 - 300 MPa in Ed's pictures as that can' be true? Where are max and min labels that are showing the max stress and min stress locations? Why didn't you see it as professional modeller? Why should anyone send you model and mesh to evaluate when it is clear you don't even understand what are you looking at?
-
That max value of stress 300 MPa is well below yield strenght of 2024. Also in color scale there is no redder color than bright red...
-
Well then Jeff, how are you not seeing what is wrong in Ed's pictures? I will show you.
These pictures are exactly from the same model, same mesh, same study. Nonlinear 65MPa pressure. Ed's way of presentation first:
(https://img.aijaa.com/b/00249/15149902.jpg)
Then how it comes without modification:
(https://img.aijaa.com/b/00458/15149905.jpg)
Do they look different? Why they do look different? Why didn't you see it?
Presentation of the same result makes it. Why there is a full scale of stress ditribution between exactly 0 - 300 MPa in Ed's pictures as that can' be true? Where are max and min labels that are showing the max stress and min stress locations? Why didn't you see it as professional modeller? Why should anyone send you model and mesh to evaluate when it is clear you don't even understand what are you looking at?
Be nice. No need to be harsh. You can say a similar thing in a more collegial way. Thank you for making clear some of the inconsistencies in Ed's data.
Yes, it seems there is an issue that is being de-emphasized, or omitted. Can't be sure if it's intentional or not. (My opinion, that doesn't look good.) Which is a reason for a few sets of eyes to look at things carefully.
The yield strength of 345 MPa claimed is higher than what I used. From my sources, typical yield strength of 2024T6 is about 324 MPa, design would be to a lower value. I used 305 MPa, as a conservative estimate. I think the simulated stress of 490 from Ed is far above even the optimistic 345. Unlike some folks, my simulations to date have all been static.
Like most people, I'm trying to sort fact from fiction. Don't want to be in the middle of any brawls, technical or otherwise. Let's keep it cool and objective. That way we can continue to learn together. Thanks.
-
Then, I know there will rise additional questions. If this is true, why it didn't rupture when Marko stressed it up to 720bars? Look at the picture. There is more material around where stress doesn't rise over ultimate stregth. But it did so in one local area. And 2024 is known to be corrosion sensitive material as well as 7075. Stress of pressure plus some additional mechanical force due to dropping the gun, pressing it towards the table, bending it somehow etc will form more external forces. It is not enough that pressure vessel can withstad only pressure related forces, it needs to withstand everyting else as well that can reasonably focus on it.
Corrosion, material yeild strength cossing and time can do bad result. I'm not stating this is the reason of mentioned burst but anyway, there is considerable high risk area in this design and we all can see where it is no matter how it is modelled.
-
Then, I know there will rise additional questions. If this is true, why it didn't rupture when Marko stressed it up to 720bars? Look at the picture. There is more material around where stress doesn't rise over ultimate stregth. But it did so in one local area. And 2024 is known to be corrosion sensitive material as well as 7075. Stress of pressure plus some additional mechanical force due to dropping the gun, pressing it towards the table, bending it somehow etc will form more external forces. It is not enough that pressure vessel can withstad only pressure related forces, it needs to withstand everyting else as well that can reasonably focus on it.
Corrosion, material yeild strength cossing and time can do bad result. I'm not stating this is the reason of mentioned burst but anyway, there is considerable high risk area in this design and we all can see where it is no matter how it is modelled.
I totally agree with you here, and your observations. There's a stress riser, and some of the material may be yielding. This doesn't guarantee instant failure. 2024 and 7075 both have low corrosion resistance, this is commonly known. You are correct, the pressure vessel also needs to resist constant pressure, pressure cycling, corrosion, and outside forces like handling or dropping. The pictures did show, fracture at or near the high stress point, very near the sharp inside corner - just like nearly all the simulations have shown. Could this be coincidence? Maybe, maybe not. However, the high stress zone could be easily ameliorated, with simple techniques, with minimal loss in air volume. How much would it help? Really don't know.
There's a common experimental technique, simply called fixing what is known to be wrong and seeing what happens next. It's not terribly effective if there are multiple similar sized error contributors, because the change is very slight. But eventually, by eliminating them one by one, we can see some progress.
-
FYI, that model of mine has bottom corner radus 0.4 like usual U-drill inserts. I think it is pretty much the same as yours.
-
Bruce, could you post a picture of your mesh in the corner region. Your early pictures looked like they had a fairly uniform element size. Looking at the Freecad documentation, it looks like they have some capability to create a refined mesh in certain locations. (example from their documentation attached).
-
Bruce, could you post a picture of your mesh in the corner region. Your early pictures looked like they had a fairly uniform element size. Looking at the Freecad documentation, it looks like they have some capability to create a refined mesh in certain locations. (example from their documentation attached).
Stan, Have to laugh, I've been struggling with the meshing as we speak. I wish I knew how to do that refined meshing. Been looking for a setting to change. I can select minimum and maximum element size. When the meshing is well behaved, (and reasonable for the structure) I get ok results. There are other times when it won't mesh correctly and falls on its sword. Looks like a sw bug that I have to report.
Let me open a different model to see if I can find a sample mesh. Have to admit, my meshes are not like in the example. My mesh is varied, but doesn't vary density like your picture. It is better to have higher density where it counts, so to speak. (And less, where we don't care as much.) I will go see if I can find a way to improve this. Do recall where you saw the picture?
Edit: Found a series of functions for this purpose. Right in front of me. Probably take me a few days to get it to work the way I want.
-
FYI, that model of mine has bottom corner radus 0.4 like usual U-drill inserts. I think it is pretty much the same as yours.
Also like typical boring bar CCGT aluminum inserts. I'm using 0.4mm in the model.
-
I'm not a Freecad user (I do need to just bite the bullet and start up the learning curve). I found this tutorial for one of the two meshing tools available, You've probably seen it.
https://gmsh.info/doc/texinfo/gmsh.html#Obtaining-Gmsh (https://gmsh.info/doc/texinfo/gmsh.html#Obtaining-Gmsh)
-
The mesh zone editing is kind of primitive in FreeCAD. I can select a line, vertex or face, or a solid. Selecting the outside edge of the tube, the edge opposite to the internal stress riser worked ok. Curiously it didn't seem to get to the inside, where the stress is the highest. So I tried the inner edge, where the stress riser is, and made a zone with more refined meshing. This meshed all of the back face inside the tube, which in my mind, isn't necessary. It's making the model too big. I won't be able to simulate it.
Last run, I used up all my RAM and all my swap. 32GB RAM, 28GB swap. Took a long time, even with SSD. So, I will need to cut the model and exploit symmetry. This was on my "toy model". Frustratingly, can't get my realistic model to mesh at all. I'll figure it out...
Stan, not 1 hour ago, I was reading that link...
Took me a solid three weeks to learn FreeCAD, at least the basics. Warts and all, it has been well worth it. Didn't have any significant 3d experience, so it was a tough week, after that it wasn't bad.
-
FYI, that model of mine has bottom corner radus 0.4 like usual U-drill inserts. I think it is pretty much the same as yours.
Also like typical boring bar CCGT aluminum inserts. I'm using 0.4mm in the model.
I am amazed you guys have to guess at this radius. I scanned the almost 30 page thread on this failure on the other forum and was surprised that some basic information was not provided. This radius spec should be clearly stated on the production drawing. I don't own this gun so it is academic for me. If I did, I would not be happy.
-
FYI, that model of mine has bottom corner radus 0.4 like usual U-drill inserts. I think it is pretty much the same as yours.
Also like typical boring bar CCGT aluminum inserts. I'm using 0.4mm in the model.
I am amazed you guys have to guess at this radius. I scanned the almost 30 page thread on this failure on the other forum and was surprised that some basic information was not provided. This radius spec should be clearly stated on the production drawing. I don't own this gun so it is academic for me. If I did, I would not be happy.
Most manufacturers don't publish their full drawings. Most don't hang out in public forums either. I do have to give Ed some credit for doing that. Have you seen full up manufacturing drawings from Crosman, or anyone else? Haven't looked that hard, but why would they do that? So they can be copied easily? Most have learned the hard way not to do this. Think IP theft and wholesale counterfeiting of product...
So there's some guess work going on. We figure the radius is within some common range that is available, and economical to use. 0.4 is a common radius that would have a reasonable tool life. From the photos it is obvious that the radius is quite small.
I also don't own this gun, so I have no skin in the game. Purely academic, and to learn new things. If others can learn new things and become more knowledgeable, that's a bonus.
-
Well, when your product had a catastrophic, safety related failure, and a lot of your reputation is by word of mouth on forums, Some information may be needed. No need to release the drawings, just clearly state what the number is, since it drives the safety margin.
For me academic, for the community, a little less so.
-
Well, when your product had a catastrophic, safety related failure, and a lot of your reputation is by word of mouth on forums, Some information may be needed. No need to release the drawings, just clearly state what the number is, since it drives the safety margin.
For me academic, for the community, a little less so.
Not disagreeing with you at all. That aspect of the design matters a lot.
Ed is on vacation, that's what he stated. Besides, the returned sample hasn't gone through testing, so it's a good time for him to take a break. Not commenting further, simply because it's speculative and doesn't help us do our own research or investigations.
-
One step forward, a couple backwards. Got it to mesh. There was a default setting in the mesher, that was incorrect. Found a way to change this. The checkbox was greyed out, so had to find a backdoor to change the setting. Finally found a way to do it. Then the model meshed (mostly) ok. The mesher was smart enough to make a fine mesh in the small radius zone, and in most of the floor of the cylinder. I would like to have more cells in the wall... As it stands there are 575K nodes.
The step backwards is although I generated the input mesh file, the solver seemed to have had a fault, which gave me an empty results file. I'll give it another try...
Edit: remeshed with no issue with 1mm max size cells. Should be ok for the 3.3mm wall thickness. Looks reasonable, finer mesh on the bottom as in the picture, and more cells in the walls. Trying a simulation now.
-
That band of coarse mesh, what/where is that? The transition from fine to coarse should maintain node to node connections, is that right?
-
That band of coarse mesh, what/where is that? The transition from fine to coarse should maintain node to node connections, is that right?
Thought there might be a question about that ;). It is the end of the tube which is 108mm further towards the viewer. It's hard to get a good view of this. Hard to get a nice view deep inside the tube. If I tilt the tube more, then the walls eclipse the view. Have a better mesh now.
Cell size is 1mm max now. previously it was 1.5mm. Tube wall thickness is 3.3mm. Here's a better mesh and possibly a better view. Maybe if I section the view, I can get a better view of the mesh transition. So far this hasn't been all that intuitive to do. I understand what I'd like to see, a smooth transition from fine to coarse, but its been a struggle to get that.
Edit: I think it isn't that bad. I was able to zoom into the tube and view the transition. Seems to be relatively smooth at the junction of the radiused corner. It seems the cells transition from small to larger as the mesh progresses up the tube. It's hard to tell with the foreshortening of the features due to the angle. After this simulation run, I will attempt a section view. What I really need to do is to figure out how to use symmetry. I know I can cut the model, but I was wondering if the FEA workbench could do it, or I had to edit the model. Haven't found the magic buttons for that.
-
Haven't found the magic button yet. I will have to brush up on sectioning the model to exploit symmetry. Sims are taking too long for me to make much progress. They are taking about 1hr 40 minutes, which sort of takes the wind out of my sails.
I finally got the sim to run with 0.4mm radius edge. There's stress in the radius area, but that's not where the peak stress is showing up. The sharp junction of the part with the o-ring with the pressure tube is showing up above yield point, the 0.4mm radius has cut down the stress to 75 MPa or so. The output vtk export file is 328MB. I will look at the file in Paraview to see if I can extract more useful information. Unfortunately, I hadn't bothered to put in the o-ring groove. Didn't think anything exciting was near there. So much for intuition.
I put a fixed constraint (red) at the end of the o-ring section, which shows up as green. The tube is pressurized to 105 MPa. Peak stress is 455 MPa, which is above the yield point of 2024. Ed uses 347, I prefer a more conservative 305.
That's what I have so far. Been spending a bit of time on this, but haven't been too productive, sorry about that.
If this were my tube, (and if I believed my results) I'd want to make sure that junction where the peak stress is would have a radius as well. As far as trust of the results, I'm not there yet. Still learning as I'm going along.
-
Bruce, in your model, is the left (threaded) side of the tube open so the pressure does not create any axial stress in the tube?
-
Bruce, in your model, is the left (threaded) side of the tube open so the pressure does not create any axial stress in the tube?
The tube is open but there's constant pressure of 105 MPa radially in the HPA section, and the same pressure on both the flat bottom and the inside radius section. So there's an axial component of pressure pushing towards the fixed constraint.
I used to have a fixed constraint at the end of the tube near the threads holding it static axially compared to the other end. I dropped it because of having so much trouble with getting anything to work, so I simplified things. I could add it back, if necessary.
Here is a graphic. The pressure constraints are the inside cylinder walls out to the dotted line, towards the right, and towards the radius ring on the inside. Hope that helps explain it a little better. Forgive my hand graphics. Fixed constraint is on the far right side on the circular face of the solid piece.
-
I added a 1mm radius to the outside section, and made the inside region a 3.3mm radius, which is the wall thickness. This should be a lower stress design, at least in those regions.
-
When the mesh isn't ridiculous, ie, forced very small by very small radii, the mesh is reasonable, and the simulation only takes 12 minutes. I can deal with that.
With the inside corner in the tube, and the small radius on the external support on the left (1mm) at 105MPa, the maximum von Mises stress is 220 MPa! Which is well under the yield point of 2024. Seems good, is it too good?
With the previous sim (small radii) the value was 455 MPa.
-
I’ve not messed with fea but I would think putting the constraint on that end puts it into compression stress at that end.
If the constraint was placed at the threads, it puts the tube into tension (which it doesn’t appear to do now). And we know the tube is definitely in tension.
Dave
-
I’ve not messed with fea but I would think putting the constraint on that end puts it into compression stress at that end.
If the constraint was placed at the threads, it puts the tube into tension (which it doesn’t appear to do now). And we know the tube is definitely in tension.
Dave
Food for thought. Not sure how to do this just yet. Here is a diagram showing where the fixed constraints are. Currently there is no plug on the chamber to exert force towards the left on the threads. There is a constant pressure outwards in the HPA region, but none to the left. See the attached diagram. Unfortunately the actual display in FreeCAD of the constraints is not photogenic, and would lead to more confusion. The developers need to work on that, in my opinion. The dotted line is merely cosmetic, but there is no radial pressure to the left of that line, as an o-ring isolates the pressure. There's clearly an axial outward force on the plug.
-
I have received some tips on how to reduce the model size, which should help. Hope to get some answers on better use of the constraints. My choice of constraints may not have been optimum. Slowly getting there. Still need some feedback on modeling the effects of the plug on the threads.
-
The analysts I worked with often used RBE2 and RBE3 (rigid beam elements in NASTRAN) to constrain something like the open end of the tube (often with a wagon wheel of elements to the constraint point). Unfortunately I could not find an equivalent in Freecad. Here is a discussion on implementation of virtual elements.
https://forum.freecad.org/viewtopic.php?t=42164&start=30 (https://forum.freecad.org/viewtopic.php?t=42164&start=30)
Maybe add a disk to the left of the threads and use the ConstraintContact or maybe ConstraintTie to attach it to the end of the tube. The disk itself would then be grounded. You could give the disk some artificial properties to control its deformation if needed.
https://wiki.freecad.org/FEM_ConstraintTie (https://wiki.freecad.org/FEM_ConstraintTie)
https://wiki.freecad.org/FEM_ConstraintContact (https://wiki.freecad.org/FEM_ConstraintContact)
-
The analysts I worked with often used RBE2 and RBE3 (rigid beam elements in NASTRAN) to constrain something like the open end of the tube (often with a wagon wheel of elements to the constraint point). Unfortunately I could not find an equivalent in Freecad. Here is a discussion on implementation of virtual elements.
https://forum.freecad.org/viewtopic.php?t=42164&start=30 (https://forum.freecad.org/viewtopic.php?t=42164&start=30)
Maybe add a disk to the left of the threads and use the ConstraintContact or maybe ConstraintTie to attach it to the end of the tube. The disk itself would then be grounded. You could give the disk some artificial properties to control its deformation if needed.
https://wiki.freecad.org/FEM_ConstraintTie (https://wiki.freecad.org/FEM_ConstraintTie)
https://wiki.freecad.org/FEM_ConstraintContact (https://wiki.freecad.org/FEM_ConstraintContact)
I will have to study that. Thanks. In the meantime, found a simply way to reduce the model size by 4. Here's the mesh and some of the constraints. This is an earlier model with the 0.4mm radius inside corner and no radius of the solid cylinder where it butts against the HPA section. The zone on the left is at 100 KPa, then the HPA section is at
30 MPa. There are displacement constraints rather than fixed constraints. The mesh is pretty fine, and increases in density by the inside corner.
A simulation shows the max stress (ignoring the thread area) is 211 MPa. Here are some of the stresses and the mesh. 2024T6 aluminum. Stress in the corner and the junction of the solid cylinder to the HPA section. More or less what one would expect. The blue solid arrows show the pressure.
-
At 105 MPa, max stress is 740 MPa for 2024. Tube displacement magnitude is 0.278mm. Stress is well above yield. HPA balloons outwards, pulls on plug, everything distorts like mad. You can see the original location and the 100x magnified displacement. Well past the ultimate tensile strength. That being said, I'm not sure this is accurate - but it is sobering. Simulations can lie, depending on how the problem is set up.
-
At 3X over pressure (90 MPa) in 7075, with a 3.3mm wall and 3.3mm inside radius, the peak stress is where you would think it should be. The other stress riser was toned down at the junction of the solid by adding a 3mm fillet. Peak stress is at 526 MPa, which is at least close to 7075T6 typical tensile yield strength 503 MPa. So even with these mods, 7075 is not achieving a 3x safety factor to yield.
But the 3.3mm radius eliminated the stress riser completely. At least this is getting easier to do. Simulations are thankfully relatively short now. Easier to see as well.
-
Excellent progress.... You have to like it when results make sense....
Bob
-
Nice results.
Typically for cylindrical (thin wall) pressure vessels, the axial stress is 1/2 of the hoop stress and does not dominate. Looking at the section cut that Marko posted, it looks like the remaining wall in the thread area is about 1/2 the thickness of the main tube wall. I could not guess what stress concentration results from cutting the threads. That area sees the axial load (but not the pressure load).
-
Barlow's formula for Internal Pressure At Minimum Yield for this cylinder works out to be 62.4 MPa, for 2024T6.
Py = 2 Sy t / do (1)
where
Py = internal pressure at minimum yield (psig, MPa)
Sy = yield strength (psi, MPa) 345 MPa
t = wall thickness (in, mm) 3.3mm
do = outside diameter (in, mm) 36.5mm
FEA shows max stress of 350.5 MPa (compared to 345 MPa yield strength of 2024T6), at a pressure of 60 MPa. They are not that far apart.
So the safety factor to yield (with the 3.3mm internal radius) would be approximately 2:1
But with a 0.4mm inside corner, the safety factor is not that good... At 60 MPa, the stress in the inside corner is 448.2 MPa, this is above 345 MPa typical yield strength.
At 48 MPa, the stress is 358 MPa. This is a safety factor to yield of about 1.6, if being generous.
If the inside corner is smaller, the safety factor to yield is even worse, which isn't surprising to anyone here.
-
Finally, if the cutter used to bore the hole had a sharp edge, like 0.2mm radius, the max stress at 33MPa pressure is 333.5 MPa, due to the sharp corner alone!
So if there was a 10% over pressure of the air charge, the stress would just about put the corner into typical yield. Corrosion would exacerbate the issue.
Interesting, indeed. Is it possible to get a measurement of that radius?
Well, that's enough work for this day...
-
First of all Barlow's is intended for "thin-wall" tubes, which is where the internal radius is greater than 10 times the wall thickness.... All of our reservoirs qualify as thick-walled pressure chambers, because the wall thickness is about 1/10th of the diameter, not 1/20th.... This requires that you use an "average diameter" when calculating the stress, that falls somewhere between the ID and the OD.... Barlow's predicts a higher stress for our reservoirs than what it actually is.... Here is an explanation, with the formulas and a calculator.... https://www.engineeringtoolbox.com/stress-thick-walled-tube-d_949.html (https://www.engineeringtoolbox.com/stress-thick-walled-tube-d_949.html)
If you input an internal radius of 14.95 mm, external radius of 18.25 mm (3.3 mm wall, 36.5 mm OD), outside pressure of 0 (gauge), and then increase the internal pressure until the hoop stress at the ID (where it is highest) equals 345 MPa (the Yield strength of 2024-T3 aluminum), that occurs at 67.9 MPa.... Interestingly, the axial stress (acting longitudinally on the tube wall, because of the force on the ends) is only 139 MPa.... If we use the Tensile strength (483 MPa), that occurs at an internal pressure of 95 MPa....
If you want a safety margin of 3:1 to Yield with 2024-T3, the MSWP is only (67.9/3) = 22.6 MPa.... Looking at it the other way, the safety margin to Yield at 30 MPa for the hoop strength is (67.9/30) = 2.26:1.... If we use the Tensile strength (483 MPa) the MSWP increases to (95/3) = 31.7 MPa, a safety margin to burst of (95/30) = 3.17:1.... This does NOT include any additional stress due to a square corner between the tube wall and the end.... That is where FEA comes in.... I personally don't think that the 3.3 mm wall is the culprit here, it is the lack of a radius in the inside corner....
Bob
-
@rsterne, Bob, no arguments from me. Dragging out Barlow's formula was only meant to show similar answers, despite not being applicable. There was no intention of saying that the formula was correct for this configuration.
I'm merely attempting to do the best I can, all while coming up to speed with the firehose of information. Your practical experience dwarfs mine. I'm willing to put in a little time to learn and add to my skills. This was a fun project to learn about this.
The sharp corner in the tube causes huge stress risers and unnecessarily reduces the mswp of the assembly. A radius of about the wall thickness reduces the stress so that the interior cylindrical tube walls are the dominant stressed item. We are on the same page. If the radius of the boring insert used to drill the tube was not controlled by specification, it could result in tubes with quite variable mswp. That's an inference on my part, based on my FEA results.
This paragraph is more speculative. Missing anodizing could allow corrosion to create micro radii in the corner region which could further enable yield. Don't know that that happened, but corrosion in that stress region, could cause stresses to increase there, eventually leading to cracking. But I will leave validation or denial of those thoughts to others more skilled in the art than myself.
Thanks for the link to Barlow's. Appreciate it.
I used the measurements that Marko supplied me. With his permission, I could send you my FreeCAD model, if you want to look at it. @MJP, may I send the model to Bob Sterne?
-
If you input an internal radius of 14.95 mm, external radius of 18.25 mm (3.3 mm wall, 36.5 mm OD), outside pressure of 0 (gauge), and then increase the internal pressure until the hoop stress at the ID (where it is highest) equals 345 MPa (the Yield strength of 2024-T3 aluminum), that occurs at 67.9 MPa.... Interestingly, the axial stress (acting longitudinally on the tube wall, because of the force on the ends) is only 139 MPa.... If we use the Tensile strength (483 MPa), that occurs at an internal pressure of 95 MPa....
Bob
I tried to radius the inside corner as best I could to almost 14.95 mm, for the existing model. Due to how I constructed the model, I could not achieve that. I did a 14mm radius, with a small 1.8mm flat spot. I had to do that, or I had a poorly behaved mesh. At 67.9 MPa pressure, I see a hoop stress of 396.8 MPa, which is similar to what you calculate. There's little stress on the 1.8mm flat spot. It was kind of lazy, but I didn't want to redraw the whole model this morning. Not saying I did everything correctly. There's some screen aliasing on the display (seen as the uncolored area) but the underlying mesh completed with no errors, and the simulation likewise shows no errors. I have attached, with and without grid. Dominant stress is in the hoop. We don't need to have such a space consuming radius, the 3.3mm radius I have show previously works rather well. I suspect 2mm isn't that bad either. These simulations are now taking about 10-30 seconds depending on how fine an average mesh is required, which isn't bad at all.
Bruce
Edit: Reverting to 3.3mm radius shows almost identical maximum stress of 396.9 MPa, with the maximum being in the hoop. 2024T3, same model as above, only changed the radius. 2mm radius is also fine. Max hoop stress is 396.7 MPa. One can see more stress in the corner, but it is well below yield.
-
As a matter of fact, even a 1mm radius isn't terrible. Yes, there's stress in the corner showing up, but the dominant stress is in the hoop. For 67.9MPa, 2024T3, the max stress is 397.1 MPa. Personally, I'd feel more comfortable with 2mm.
-
1.5mm radius keeps the corner stress under 297 MPa, and leaves the hoop stress the same as before. It's a little bit above yield point at 397 MPa.
Think the real issue is, 2024T3 isn't all that strong. And having a corner radius < 1.5mm adds a dominant stress riser in the corner. Input pressure was 67.9MPa.
With a corner radius of 1.5mm and an input pressure of 60 MPa, I get a stress of 350.7 MPa. Lets call that the yield point, close enough to 345 MPa. So this tube has (ignoring the threads!!!!!) a safety factor to yield of 2:1, if and only if the corner radius >= 1.5mm. The tube that Marko originally sectioned had much sharper corners than 1.5mm.
-
At 0.2mm radius is nearly at yield at 34 MPa. Inside corner stress is 344 MPa, close enough to 345 MPa. That's a safety factor of 1.133:1 to yield = bad news.
So if your pressure cylinder has a tight sharp inside corner on the order of 0.2mm radius, I'd not use it, at least not at rated pressure. An overfill of only 13% puts that inside corner into yield. Is your pressure gauge good to 10% absolute accuracy? Probably won't be a problem initially, but over time, pressure cycling, corrosion, it could become an issue.
Learned a lot doing this. Hope it was of some help to people, even if it was nothing besides confirming knowledge.
Bruce
-
More data more knowledge is always good.
I will see when time permits if I can destroy the remaining yielded cylinder.
Just realized that I have a pump capable of 2400bar in my commonrail injector test bench.
Need to make injector fitting in to the cylinder and a bleed port to get any air out.
I don't have a analogue gauge to measure that pressure but I can monitor rail pressure sensor voltage to where it peaks before something gives up.
Marko
-
Bruce, great work! That mesh looks really good.
I wonder about the axial load. It would not affect the hoop stress in the middle of the tube but I'm not sure if it affects the corner stress. Even a simple constraint at the thread end may be OK by the time it gets to the corner.
Marko, would it be possible to add strain gages to the tube for the destructive test?
-
Thanks, Stan. Still trying to figure out how to set up a non linear simulation in FreeCAD. It's kind of silly, but I don't understand the input data format. I have to enter the stress strain curve for the material, but the format shown in an example FEM FreeCAD file is unknown to me. Just an example, but no words describing the details. Details that are undoubtedly known by practitioners of the art. Probably obvious to someone with strong mechanical background, but as you can tell, I just starting to learn this.
-
Well, got the non-linear formatting sorted out. I had it all wrong. :-[
The data format for the non-linear is kind of strange (to me) but, it is a plot of the breakpoints of the stress strain curve, but the first breakpoint strain value is set to 0.
Trying again. I have 8 cores running on the problem now. Maybe this time the sim might converge. Taking it's sweet time, it's been over 27 minutes...
-
Foo, hit timeout before I could finish editing!
Edit: Finally finished, (about 1/2 hour) but I'm trying to interpret the results. Quite a few of the simulations did not converge, so this took a while. The sim generated 13 unique data sets! The model/data file is now 435 MB. Prior to this non-linear sim, it was a mere 19 MB. Is the idea to sift through the data to determine if the Equivalent Plastic Strain greater than some value? (3%?) This is the cylinder with 0.4mm radius, at 75 MPa, using two points for non-linear 2024T3. My figure shows the equivalent plastic strain.
I used the following points:
344.74, 0
358.53, 0.005
[MPa, unit less]
Got the material data from: https://icme.hpc.msstate.edu/mediawiki/index.php/Aluminum_2024-T3_Stress-Strain_and_Fatigue_Life_Data.html figure 10, for tension.
-
Good job getting Freecad to run non linear solutions. I think with a .4mm flaw size, this ends up being a fracture mechanics research project. Just reading the Wiki page should show how much fun that would be.
I can't understand why the manufacturer would try to defend using material yield to meet safety margins instead of the simple 3 mm fillet that solves the problem with straight forward linear analysis. At some point, maybe they should just stop digging the hole.
Great work.
-
Good job getting Freecad to run non linear solutions. I think with a .4mm flaw size, this ends up being a fracture mechanics research project. Just reading the Wiki page should show how much fun that would be.
I can't understand why the manufacturer would try to defend using material yield to meet safety margins instead of the simple 3 mm fillet that solves the problem with straight forward linear analysis. At some point, maybe they should just stop digging the hole.
Great work.
Thanks, some of this stuff (documentation) takes a while to ferret out. Like it's nowhere in the docs. Had to point blank ask the question about the data formatting. A gentleman on the FreeCAD forum told me that at 75 MPa, my simulation wasn't really converging. He suggested a 70 MPa value, saying that at 75 MPa, it's perhaps this thing would have blown up. Honestly, don't know if that is true, or he was just trying to have me be extra cautious. He did say plastic material analysis is forbidden (in the EU) for pressurized vessels over the whole structure (for good reasons). That I believe.
Here's a non-linear simulation at 70 MPa, showing the cylinder at yield stress along nearly the whole HPA area, with the stress above UTS in the radius. Pretty scary, at least to my ignorant self. Perhaps, this model isn't constrained correctly, or incorrectly implemented, but it is an eye opener. This took 3 minutes, with two point nonlinearity.
When you do the problem correctly, the file size seems to decrease, thankfully. Now at 230MB...
-
It may be interesting to run the 30MPa basic fill pressure case and see how much is above yield.
I think your constraints are OK for what you are doing. This is an internal loads case. Constraining the model with a 6 degree of freedom connection to ground is sufficient. I think you have that on the right side of the o-ring block. As you have it, there is an artificial compression force on the o-ring block. That is not the high stress area. To be more representative you could add a cap disk to the threaded end, join it to your model as mentioned earlier and then ground your model there. That would add the axial load to the tube and remove the compression on the o-ring block. This may change the stress in the fillet.
-
It may be interesting to run the 30MPa basic fill pressure case and see how much is above yield.
I think your constraints are OK for what you are doing. This is an internal loads case. Constraining the model with a 6 degree of freedom connection to ground is sufficient. I think you have that on the right side of the o-ring block. As you have it, there is an artificial compression force on the o-ring block. That is not the high stress area. To be more representative you could add a cap disk to the threaded end, join it to your model as mentioned earlier and then ground your model there. That would add the axial load to the tube and remove the compression on the o-ring block. This may change the stress in the fillet.
Good stuff. I will try that out in a couple of days.