less than impressed with Creo Sim 2.0

[scollins]

I've been trying to deal with a 20 pc. assy., but currently crashing. I cannot post pics nor assy/prt files. This is essentially a flat plate w/both simulated fasteners and solid screws into a fixed mounting structure. Plate has a pressure load applied. The fastener preload iteration took 8 hrs to run on 'quick check'...

I need this to RUN!!!!!!!!!!!!!!!!!!!!!!

At this point, no preload on the solid screws is necessary

I feel this has taken far too much time....approx. ~100k elements, (if I can even get it to complete the mesh).

To prevent chattering, I've tried to match tols by switching all part accuracies from 'relative' to 'absolute'. Using def. tol of 1e-4,

refined meshing on rounds, cbores, thru holes of interest...thru Autogem....used a lot of 'Max. Elem Size' and 'Exclude Singularties' @ re-entrant<150 deg.....

Nodes? I have laid down some of these - There seem to be directional arrows....right click in collection box and "fix"...did this....

Autogem Settings - "detailed fillet modeling" is checked...

There is a skeleton with curves I used to trace the sim region...this seem ok....

I've gone down to the part level and refined meshes there, am intending on using these piece part meshes at the top level...am I wrong to assume this?

How is it that I can't get this to kick, but every little demo and presentation is always just sunshine & smooth sailing....

Now - the ANSYS group is chomping at the bit to get their hands on this and I have no grounds to hold them at bay..I have until Fri. to get this assy. running...

btw- brand new M6800 w/32Gb...so it's not the hardware...

cpu 'use all'

Q: Comments? methods?

Thanks for your attention and review..

Sean

This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

[scollins]

Thanks for the response...yeah I thought this should be easier, if it's just the plate, no problem but a top assy not so good...chewing up a lot of time, will go to SPA. Yes..contacts...a number of them

The stresses in the plate & stress in simulated fasteners (10X) are my primary interest. Not interested in fixture stresses, mount is fixed in 3-dirs...also not interested in some fastened components..but I need them for the assoc. weight.

yes.. plate assy. is "screwed" to a fixture, so I can get fastener stresses...

addt'l info...

both plate & fixture are made of 2 materials, so I merged the plate into one .prt and fixture piece into one .prt to produce a 2 part assy. and be able to use simulated fasteners.

The solid fasteners are just there for contact, I bonded them to the fixture. Preload on these would be nice for completeness, but not necessary.

[dschenken]

Best suggestion I can make is to sneak up on it. Use cuts to remove most of the geometry and see if one small piece with one fastener works. Move the cut back and see when it stops working right.

Had an Ansys failure with heat transfer - put in a million watts per square inch to get a .1F rise in temp on a tiny fin. Turned out Ansys never tried non-metric units with that module in their testing and it didn't work otherwise.

So. Convert the problem into one that is too simple to fail and work from there.

[scollins]

I'm working on it now, messing with the Geo Tol...not having any luck.

Previously, I had suppressed piece parts and got it to run, albeit a long runtime, and I have suppressed chamfers, holes, rounds on various, but now I need the assy to run!

[346gnu]

Hi Sean,

What I understand of your model is not frightening at all and Creo should eat it.

Post your diagnostics.

A technique we use when debugging awkward contact problems is to switch to MPA and set the max edge order to 1 (and sometimes limit the number of contact irerations as the default is 200 I think). This makes each failed run as quick as possible.

As Steven Dunker said, absolutely no mesh refinements until it runs. More elements=slower to fail

Yes, for the moment remove (supress) all that you can to minimise the element count.

If failure is due to insufficiently constrained take a methodical approach and put individual and fully constrained displacement constraint on each and every component. Remove these 1 by 1 until the problem returns. (one cannot use modal to identify insufficiently constrained components if contact is used. (quicker iteration method is bisection method if you know this)

If everything is constrained and it still fails insufficiently constrained then there are 2 more likely explanations

1. Advanced fastener interface regions and/or top regions overlap tangent lines or run off the edge of a component.

2. Model accuracies causing elements to be created in daft places such as in the middle of holes and completely disconnect from main mesh. Use boundary faces to assist (though less effective in big models with lots going on)

If using solid fasteners temporarily swap for the (now old) 'advanced' fasteners. Solid fasteners introduce a new bag of issues re contacts and additional DOF's to manage.

Post your diagnotics

If I think of anything further ...

Regards

Charles

[scollins]

Charles - Thanks for your response...

Haven't run it yet..but have marched thru the piece parts and adjusted loosest Geo Tol. for each piece such that they generate min elements and have no diagnostic errors.

A larger question would be ...what is the driving Geo Tol...

Does the subassy Geo tol override the piece part tol for meshing?

Sean

[346gnu]

Sean,

I rarely play with the tolerances unless there is significantly different values or things are hard to mesh.

If it meshes problems may be elsewhere.

I regularly build and run assemblies with 10-50 fasteners and 10-20 major components and many many contacts and 99% of the time it's user error when something doesn't work.

The diagnostics referred to are those from the actual analysis run, not the mesher.

Regards

Charles

[sdensberger]

Couple pointers that you can use to diagnois your problem:

1. To help narrow down whether a meshing problem is due to a tolerance difference between components or due to geometry, suppress all interfaces that you've defined and change the default model setting to free. If the model meshes without a problem, then your issue is likely an interface one.
2. It's generally best that you don't add in any mesh controls until after you've gotten your model to run.
3. I don't know for certain (since I can't look at your model), but 100k elements sounds like waaay too many. Remember, Mechanica is a p-version FEA code; chunky elements with large aspect ratios (30:1) can still give very good results.
4. I'm not sure if you're using solid geometry for your fasteners or if you're using idealized fasteners via the fastener tool in Mechanica, but if it's the former, then make sure that the fastener and nut can't 'spin' in place. This rigid body motion will result in a singular stiffness matrix.
5. It's typically best to add in a couple components at a time, do your pre-processing work on them, mesh and run, and then add in more components.
6. You can run a modal analysis with the rigid body mode box checked to see if any of your components are undergoing rigid body motion.

[scollins]

Thanks Shaun,

yes...100k is wayy too many...

I had a simpler model running, added mesh control, then had to add components...then snags that I'm trying to get over.

I've been keeping the diagnostics box clear of edges/surface removals flags by modifying the Geo Tol. Settings.

I will double check the solid fasteners that they are set in 3-dirs.

I'm getting some degenerate surfaces

Sean

[scollins]

suppressed the Autogems....back to crashing the program.

Thanks for you review and assistance..

Sean

[sdensberger]

Crashes as in straight to the desktop?

[scollins]

yes

[sdensberger]

This sounds like a corrupted file issue; removing mesh controls shouldn't cause a crash to desktop. Of the 20 parts in your assembly, are any of them patterned? If so, then your best bet might be to re-create the assembly and modify how the geometry is represented to speed the pre-processing phase up.

[scollins]

material...

each piece part has it's own material assignment..

do I need to re-assign in the subassy...I thought this should carry up...

[sdensberger]

You shouldn't; material assignments will carry up from lower level assemblies or parts.

[neomechanikos]

I've had it crash to desktop before because somebody had messed with the material properties, modulus in particular. Double check your material properties.

On another occasion another assembly wouldn't mesh properly and error messages lead me to believe it was accuracy mismatch. Trying to match accuracy and change tolerances lead to crashes. Turns out it was bad model geometry. I corrected a few geometry checks in a part then got the accuracies close and all ran good after that.

What build are you on?

[scollins]

build M050...I don't have any geom checks....the Geo Tol settings have helped at the part level, but not at the master assy level.

materials are ok then, I have PR, E & density for all materials...

my understanding is the Geo Tol settings at the top level assy. overrides the subassy & part level settings.

Guess who just got instructed to use his ANSYS...

Sean

[scollins]

Better news...the top assy has run (SPA) ...attached are files...

I modified the Geo Tol FROM: 1e-4 & 0.86 deg. TO: 1e-3 & 1 deg., iterates faster now. Most Autogems are still suppressed.

Still can't get my 3 simulated "Primary" fasteners to come in...

was thinking...should Autogem limits be reduced and Geo Tol be increased?

Sean

[346gnu]

A quick look

From the .rpt file

One immediate issue you have to look at ...

At the top of the .rpt file :

** Warning: Two faces (DBIDs: 83341938 & 83208508) on opposite

surfaces in a contact (DBID: 82855602) are

connected at a node (DBID: 82789300). This prevents

the surfaces from moving completely apart during

a contact analysis. If this is not what you

intended, please edit your model appropriately.

Probably means that the boundary of one of your contact regions is is attached to the opposite surface when it possibly should be free to slide/separate, This will mean load will be transferred through these nodes and the structure not move as it should. Local fastener forces will be affected.

One cause of this, for example, is the creation of a surface/volume region after the definition of a contact. The original contact now has to become 2 contacts and you only defined 1.

Review the run diagnostics, these will appear as orange dots. Select one and see what is highlighted in the model. You then have to reverse engineer the reason to fix it.

Ignore the following for now.

*** Warning: Large deformation and/or strain detected during contact analysis.

More accurate results may be obtained if 'Calculate Large Deformations' is selected.

Switching on LDA will cause a ramp up in analysis time you don't need at the moment. Besides, it could be inappropriate is material strains are low and the large movement is due to sliding.

The fastener forces. One shouldn't expect more than a few percent variation from preload values

Buffer# - 1.7e4 - ish ok?

Cylinder 312 to 2.3e4 - quite a range,,, suspicious

secondary - 712 to 1.6e3 ....mmmmmmmm

clamp3, insert1&2, promary4,5,6, secondary 3,5,6 small numbers, likely to be wrong (if these are fasteners).

tele# - all 7.5e3 -ish ok?

2. Causes of smaller than expected fastener tensions:

-Local contact region boundaries sticking to opposite surface (above)?

-Fastener surface regions (created by the software) running off the edge of a component/into tangent lines (rounds) overlapping neighbouring fastener regions.

Analysis time is reasonable.

From the .pas file, the residual norm 'collapses' in a well behaved manner, the contact solution seems good.