I'm trying to simulate the insertion of a metal "y"seal (yellow) into a gland (blue) to seal around a rod (metallic color). I'm a seasoned FEA user, but this is just past the edges of what I've done before, so I'm working out how to do it correctly. I want to see if this can be done in Creo 3.0. I thought I'd post the question to see if someone more knowledgeable than myself can provide some insight on what I'm doing wrong.
I've started with a 2D axisymmetric analysis, shown below, and plan on doing a 3D model as a slice. The basic details are;
-Rod and gland are fixed in X & Y
-Y-seal is fixed in X, fixed displacement in Y direction of 0.15 in. to make it land in the bottom of the gland.
-Basic mat'l properties for now, steel rod and Y-seal, SS gland.
-Contact analysis defined for edges (since its 2D axisymm) that come in contact, finite friction, mu=0.2.
-Nonlinear analysis, 10 equal steps to show some resolution.
-Model runs in ~10 min, SPA, initial mesh for pass 1 is chunky but I let it do some automatic mesh refinement on pass 2 and it looks pretty detailed where its needed.
The 2D model runs and shows results somewhat like I'd expect. I expect to see the edge of the y-seal ride up on the gland and rod and NOT penetrate them. I do see some movement of the y-seal arms as it contacts, but it does penetrate the two other parts slightly. I'm not sure why it does this, but it makes me think I'm missing something.There are enough nodes in pass 2 that its not simply element passing thru element without nodal contact.
I've attached a zip file of the parts used in the assembly. Does anyone have any ideas/suggestions? Am I asking to much of Creo, or just myself?
Thanks in advance!
A couple things:
- It looks like you're using linear-elastic materials properties (which if fine when developing your model), but If I recall correctly, Simulate cannot do large-displacement formulation and plasticity in an 2D axisymmetric analysis (maybe they added this in 3.0; not sure). If this is the case, then you'll need to switch to a 3D wedge model.
- For an axisymmetric set of boundary conditions (whether 2D or 3D), you do not need a constrain in the X-direction (unless there's additional structure that isn't show in the model that'd prevent X-direction motion). Any motion in the X-direction develops strains in the theta-direction.
- Something you might want to consider is moving the Y-seal just shy of coming into contact with the glad, and use an interpenetration initialization step. The gap should be as small as possible, but large enough to allow the frictional forces to build to the maximum allowed by the static coefficient of friction (if you think these forces really matter). This should cut down on the overall run-time of your analysis and won't effect your final results (as I understand what you're trying to simulate). This might also remove the need for large-displacement formulation.
- With large-displacement formulation removed (and while still using linear-elastic material properties), you can run a MPA analysis to ensure that your mesh is good enough to converge. Once you add in non-linear material responses or large-displacement formulation, you'll be restricted to just SPA.
- Contact in Creo is handled via a Penalty Method, so there will always be a small amount of penetration occurring. What Creo is essentially doing is adjusting the stiffness of springs between pairs of contact surfaces until a predetermined residual is reached. As such, the only way to have zero penetration would be to have an infinitely stiff spring, which cannot be done. Some other FEA codes will use a Lagrange Multiplier Method, which exactly enforces the contact condition.
- As far as whether this is too much for Creo depends on what you're trying to get answer-wise from this analysis and how important the answer is. Can you provide a little more background?
Thanks for the great comments. I'm still new to Creo, having been forced by the man to switch from SolidWorks. Most of what I had done to that point on this FEA model was still "quick and dirty", though second or third cut.
-I started with a 2D model to see if that was enough. I'll have to dig around to see if LD & plasticity can't be handled in 2D, I don't know that I saw/read that anywhere. I have a 3D model, but wanted to compare the differences between 2D & 3D to see what the costs/benefits were.
-I should have known better about the X axis, think I played with that on & off.
-The y-seal is very short ~0.1 inches, so a smaller translation range makes better sense.
-I suspected that there was some enforcement going on as the part moves a little as I'd expect under "no pentration". Luckily I just spent the weekend reading over contact methods in Ansys so I'm aware of the 2-3 different methods of enforcing contact.
-Answer-wise, I'm trying to extend my FEA capabilities past simple linear models with some confidence. We've asked two manufacturers for FEA on their products, and the answers have been pretty simplistic and obviously off. We do these types of products often, and would like to develop some in-house knowledge to do this analysis, if its possible. To that end I'm trying to understand what we can do in Creo and where the boundaries are. The only decent manual I've been able to find is Roger Toogood's, and while its a great basic primer it doesn't dive into many of the finer points.
Thanks for all you insights!!
So linear-elastic stuff, Simulate is a decent FEA package to use. For non-linear stuff, it starts to get a little iffy, but it's still possible. Stuff like insertion forces shouldn't be an issue, but getting accurate stresses will be tricky.
I'm running your model now, did some modifications already: Changed all to metric (I don't understand the fun in these imperial units), added elasto-plastic material properties, defined contact surfaces and a bit of friction. Am now running a 90 degree model, with a prescribed displacement and a measure to determine the load.
Will get back top you when the job's done.
Thank You! As for imperial units, old habits die hard.
Let me know what you come up with, and any suggestions you have on how to properly set this up and run it next time would be a HUGE help.
Why 90 degrees and not a small wedge? It also looks like you're constraining the R-direction on the top surface of the Y-seal; this isn't realistic.
Small wedge requires cylindrical coordinate system for the constraints, which gets you into trouble with the reaction load measure.
You are right about the constraint on the top, that is wrong, sorry!
I'm re-running it, now only axial displacement prescribed.
True, but you could use a link, simple spring, and a measure to get the reaction force if you really wanted it. It'd be much more efficient compared to a larger model.
Have you looked at this discussion.
Solved: User need help with Simulation setup. - PTC Community
I thought this was going to be an easy one.
Looks not too bad, but I keep on having interference. The y-seal doesn't deform enough and I don't understand why. I tried several things: refining, increasing accuracy etc. Doesn't work. Is it because this thing is tiny? (about 3 mm diameter). I'm showing the results for the linear elastic model, the plastic model gives better stresses, but still there is undesired interference.
Can any of the other readers in this post tell me what I'm doing wrong?
I've added the most simple one I did, linear elastic, default mesh. runs just a few minutes.
In that last image, is the displacement scale set to 1? What does your mesh look like? Keep in mind that Simulate is uses a penalty method for contact, so there will always be some level of penetration.
the scale is indeed 1. I've tried several levels of mesh refinement, but do not see any influence on the displacement results. I find the penetration large compared to relevant geometry dimensions
I was able to get similar results. I did see the y-seal push away from the rod and gland, as you would expect, but like you mentioned the amount of penetration still seemed large compared to the overall size. I did see a reduction in penetration from pass 1 to pass 2 when I checked the "allow mesh refinement" box. If you show the element edges on the FEA results you see that mesh refinement puts more elements in the contact zone on pass 2, as you'd expect. Maybe the answer is to just mesh the heck out of the contact region and look for improvement?
ou could try with the heck, but it should mnot be necessary
How are the contact-pairs defined in your model? I don't have 3.0, so I can't check you files. You could also try adjusting the configuration parameter "sim_contact_penetration" and see if that helps.