Maybe someone can help me with this -- the only way that I have been able to run this study is with a global bonded contact and no contact sets specified. Once I add No Penetration contact sets, the model repeatedly fails. I've tried changing the mesh size, the time step, the connectors, and anything else that seems related, and have had no luck. I was wondering if anyone could give any insight, or maybe run the study to determine what direction I should take. Thank you for your time.
--Bryson
Well, the bolt definition also failed eventually (just had to wait for it to subdivide time steps to fail to converge).
I simplified the model down to the 3 mounts and the first bracket. It complained about the contact definition during the solve.
So I redefined the contact using the bracket as the first surface and the 3 mounting faces as the second set of surfaces.
And hey presto, it starts solving.
An improvement for 2009 was that the surface order was not meant to impact the contact definition. Obviously it still is sensitive to it in some situations.
So try that on your model and see if it resolve the issue
Cheers,
Ian
Ian,
I really appreciate your help with this -- I've been struggling with this particular study for awhile now. However, I tried the things that you suggested and am still getting failures. Here is the route that I took:
Starting with the original assembly (all components included)
Reversed the order of the no penetration contact set between the bracket and 3 mounting plates -- First Step Error
Reversed the order of the no penetration contact set between the bracket and the monitor mount -- First Step Error
Reversed the order of the bonded contact set between the monitor mount and the monitor -- First Step Error
Supressed the monitor mount and monitor -- First Step Error
Re-reversed the order of the no penetration contact set between the bracket and 3 mounting plates -- First Step Error
Then, I created a new study including all components so that I could create everything new. Instead of pins, I created bolted connectors (1/4" shank, 1/2" head diameter, alloy steel, tight fit cleared, 96 in.lb preload) at all 17 locations.
Ran the study (bolt connectors, all components included) -- "Bolt Connector surface not defined"
Supressed the monitor mount and monitor -- "Bolt Connector surface not defined"
Then, I unzipped the file that I uploaded, just in case there was some slight difference in the model that you used.
Supressed the monitor mount and monitor and reversed the order of the no penetration contact set between the bracket and mounting plates, and I got an error message saying "Security device is not responding; please install security device." I clicked OK to proceed with the study, and it failed on the first step again.
Any thoughts? Feel free to give these files to QA. I'm running SW 2009 SP4.1 -- thanks again for running through this.
Hi Bryson,
It appears the issue is related to the contact. Now I've done quite a few nonlinear runs in the past, but not using an acceleration loading input (I've primarily used linear dynamics for that). For parts that are moving rapidly, there can be sensitivity in the mesh when detecting penetration and I can only assume that's the real issue here. It is possible that adjusting the mesh definition is adjusting the time when there is an issue with contact so that is doesn't always occur at the first time step.
One way I was checking this was to delay the start of the acceleration profile away from time zero. I assume the loading input is the one out of Mil-Std-810E? I set up a loading to go from zero to 20g's from .01 to .021 seconds and then drop off by .022.
I have had success only in running the analysis without contacts (pins or bolts work fine for the connection laod path). I know this is not the exact replication, but it still should give you excellent insight into the dynamics. I would think this would be conservative since the loading should be higher than if the surfaces contacted each other at least for low cycle loading.
I'll see what feedback I get from QA on the issues with the contacts.
I'm trying one more run with split faces so I can get the mesh on the contacting faces similar in size (and localize the mesh refinement).
Cheers,
Ian
Correct -- it's the shock loading from MIL-STD-810G: 516.6 Procedure I and VII -- Functional Shock and Crash Hazard Shock. I actually began this study trying to start the pulse at 0.003 seconds and knocked it back to zero trying to fix the error message.
Also, I'm not having any luck with split faces and mesh controls. I tried treating everything as solids, I tried reversing the order of the contact sets, I tried using bolts (surface not defined), and I tried reversing the order in which the pin faces were selected. I even tried replacing the base excitation with a gravity load that varies with respect to time, and still haven't had any luck. I tried applying a time-dependent force to all the faces as well (even though it's not completely accurate) just to see if the acceleration load was throwing off the study, but that study failed in the first step as well.
I was able to get the model to run using split faces to provide compatible meshing at the contact areas.
3 things not in the model: Friction or you damping parameters, large displacement.
The solve took about 18 minutes, but the results look unrealistic (look at the first study) perhaps due to large displacement not being active.
keep this in a separate area on your system as I did the split faces using external references which I then broke (quick and dirty to test it out).
Hope this helps you out.
cheers,
Ian
Sounds like good news! I just started the study. I'll be back online and let you know how the study turns out in about an hour. Thanks again for all of the help.
Not sure what's happening -- the first time I ran the study, I got results that showed a pretty realistic stress distribution, but overall lower stresses than expected. It turns out that the sawtooth pulse is set to run from 10-21ms, and the study ended at 15ms. When I changed the loading to start and end earlier, the solver seems to ignore the no penetration sets. I can watch the study run in about 10 minutes, and it never locates any contact points or performs any contact iterations.
After trying several different things, I went back to the original study that i uncompressed and saved in a seperate folder and tried running it just as it was before. I'm still seeing the solver ignore the no penetration contacts, and I haven't changed anything on the study. I shut down solidworks and am going to try again later -- I figure that maybe because I copied and pasted your files, the program may be referencing incorrect information (same filename but different directories). I'll probably rename everything next time, as well as change folders. I also need to apply a material and tensile stress area to the pin connectors, so hopefully that won't mess anything up.
Also -- I noticed that the bracket has two mid-plane features in its tree. I tried editing the feature to figure out how/why they were created, but couldn't get much info as to which faces were used to make the mid-planes. I have never defined my own mid-planes when using sheet metal parts -- is this something that may cause problems in a non-linear dynamic study?
Hi Bryson,
Indeed, I am seeing that too on the large displacement model. I will look into this a little further as that does not make sense. How sure are you of your global damping terms? This is one area I'm not all that familiar with in regards to practical values.
I added gravity to my model which should force contact at time zero so will see how that goes.
The midplanes you see are an artifact of the sheetmetal midplane mapping. The program creates a midplane surface for the sheet metal and utilizes that when meshing. It should not be showing ideally, and I have not kept up with the behavior over the 2009 service packs with that aspect. Make sure you do not reference these. There no harm in hiding them. Just do not try to reference them when defining the model or you will have problems. I thought that they were meant to be hidden by default, so perhaps it's a bug or rebuild induced issue.
Cheers,
Ian
I've noticed the midplanes before and assumed they were created for the shell mesh, but they rarely stay in the feature tree. Either way, they don't seem to make a difference.
I re-downloaded your .zip file and ran your study without changing anything, and for some reason the no penetration contact seems to be ignored this time. I hadn't changed the name of the study yet, though, so I duplicated the study with a different name and adjusted the acceleration/time curve. I was hopeful because I started to see contact points, but at the end of the loading pulse the solver failed to converge while establishing contact points, and I ended up with a stress plot that I've attached to this post. The second screenshot shows the outline of the split face to give an idea of the size of this starburst.
Anyway, I just created a new study: I treated all of the components (except the monitor) as solids, applied the mesh control to all split faces, and set the loading conditions and pins just as before. It's running now, but it will probably take quite awhile.
As for Rayleigh damping coefficients, I was just guessing. I developed some formulas based off of an ANSYS Structural Analysis Guide, but I found that the guide has some conflicting information. When I use the data I've collected from a frequency study into my formulas (which I have verified with textbooks), I get a much larger alpha coefficient than beta. However, the ANSYS guide suggests that mass damping (alpha) is usually very small and can be neglected. I could try putting my calculated values into the study, but I haven't yet.
I also ran several studies with gravity involved, but this was before the mesh refinement method that you applied to these parts -- I might need to try running it that way again. This particular study I'm performing may not finish by the end of today -- it's about 10% through the total time of the study and it's been running for about 25 minutes.
Hi Bryson,
I have to say, this really seems to me like be a bug in the code. I've tried everything I know to get it to recognize the contacts with no luck.The problem is very unusual, and not something I have encountered before.
QA looked at it and are going to raise an SPR since they were unable to get the model to solve. Once I get that number I will pass it on to you.
My recommendation at this point it to avoid trying the model with contacts and go with the simplified assumption of all load transfer via the pins. At least until development identify the root cause and provide suggestions to correct the issue or a fix to the code.
I'm very sorry you've had to battle this issue and hopefully we'll get a response on what the issue is soon.
Cheers,
Ian
Ian,
Thank you for all of your help -- I appreciate you guys taking the time to look through this study. Have you attempted to run any other Non-Linear Dynamic studies using No Penetration contact sets? I have to perform studies on many of the parts we use, and almost all of them require no penetration contact conditions at the mounting points for the GFE, as well as to the vehicle. Bonded or Free contacts usually won't work because we need to analyze stresses in the connectors, and also because we must apply a shock in both directions for each axis.
I guess my question is: is the problem with the code specific to this particular case, or is it more of a global problem involving the no penetration contact set in the non-linear dynamic study? Also, do you think that trying the 2010 Beta version may alleviate some of these issues? Perhaps someone could try running the study with that software.
Thanks again for all of your help, and please don't hesitate to email me with any updates or questions.
Bryson
Hi Bryson,
Yes, I've run many nonlinear simulations with no penetration contact. Most of what I've dealt with has been solids, not shells, but I was playing with another model this morning with shells doing a nonlinear run and the contacts were detected no problem. So most likely it is model specific, not that I spotted anything out of the ordinary with the model.
The QA person looking at the problem appeared to be using 2010 code. He was running the model that failed on the first time step and had not yet run the model with the contact not being detected. I'll give that a quick whirl while waiting for feedback from him.
Cheers,
Ian
Hi Bryson,
No joy for me running the shell model in 2010, however I can run the solid variant no problems (I was able to run a solid model under 2009 as well).
I used draft elements to do a quick solve. So with 12000 elements it took 12 minutes to solve. Attached is a deflection response from the run.
Cheers,
Ian
Hi Bryson,
QA logged the SPR for the failure to solve on first time step (SPR51792). I'm waiting for feedback from development now.
Cheers,
Ian
Hi Bryson,
I took a look at your model, and it's a little puzzling why it considers it unstable.
I did the following tests:
Bonded all contacts - Model started to solve
Added rotation lock to pins (with no penetration contact) - Model still unstable
Solids instead of shells (no penetration contact) - Model still unstable
Suppressed contacts where pins are used (ie pins are only load path) - Model started to solve
So I suppressed the pins and defined bolts with a little preload and it no longer complains of stiffness singularity at time zero. With the no penetration contact, the solve time is going to be lengthy, but I'll let it chug along and see the result.
I would not have expected the pins to be an issue. The only thing I didn't try was add mass to them. However I do not feel this is necessary as the pin is just coupling certain freedoms between the 2 shells and there is more than enough pins to sufficiently restrain the parts.
If you don't mind, I can pass this on to QA to check it out.
BTW, I'm trying it out on 2009 sp4.
Cheers,
Ian