Creo Elements/Pro - Difficulty Meshing Top Level Assembly 1

[VRUGRU]

Hello,

I am using Creo Elements/Pro to build a Mechanica model of a large assembly. I am able ot mesh all the sub-assemblies and parts successfully. However, the top level assembly fails to mesh. The diagnostis window of AutoGEM lists a bunch of edges all belonging to a single part and gives me the error

"AutoGEM has detected an element incompatibility across the highlighted curve. Adding points to the curve may help. In some cases, re-creating the curve and adjacent
surfaces may be required. Could not complete creating elements
on all of the selected entities."

Has anyone in the community encountered this error? How can I resolve it.

Thank you very much.

 

[jvian]

Sounds to me like an issue with model accuracy or assembly offset constraints. It may help if you post a little more information about your scenario (i.e. what type of analysis, constraints, any contacts etc.) to better understand what may be happening but again this most often happens to me when we have an issue with part tolerances. In assembly mode look at the tolerance report to show the relative/absolute tolerances of your models. If there are large differences (i.e. orders of magnitude) then that may be your issue. Two parts of equal relative tolerance (the default in ProE) one with a large model size and one with a small model size (for example a small alignment pin in a large housing) will have difficulty meshing due to the difference in the smallest perceived edge size.

Hope that helps and good luck,

- J -

 

[VRUGRU]

Thank you jvian.

This is just a linear static analysis that I am trying to perform with several load cases. However, at this point, I am just trying to get the top level model to mesh. I have not applied any of the loads and constraints yet. Also, I have used both "end weld" features and manually created welds in the top level assembly and sub-assembly levels to capture all the connectivity details. The overlapping surfaces are treated as "free", and there is no contact defined. Connectivity is through "bonded" interfaces through the welds.

The top level tolerance report shows quite a spread. The highest part tolerance is 4.77 mm and the lowest part tolerance is 0.07 mm. All the parts have "Accuracy Type" set to "Relative" and "Accuracy Value" is set to the same for all parts (by default). I have tried changing the "Geometry Tolerance Setting" at the top level to "Absolute" and played with different numbers without any luck. I have also tried to change the part accuracy. Some parts fail to regenerate when I change their accuracy.

What would be an easy way to fix this?

Thanks again!

 

[jvian]

I am pretty sure that the accuracy difference is your problem. I ran into this frequently where our CAD modeler would not care about the accuracy on an assembly level and it would cause your described problem to me rather regularly when performing simulations. Really its the difference between a CAD model and an FEA model with the latter having to be much more robust. What ultimately had to happen was a company-wide change to the default templates used to create all parts and assemblies which set the default part accuracy to an absolute value. This does cause problems as you stated on the modeling side where regenerations would fail and the model file sizes increased but it prevented "re-modeling" just to get assemblies to mesh which saved a lot of time.

My advice is to set the part accuracies (on the part level not the assembly level) lower for the larger models and higher for the smaller models. This will bring the two closer together when viewing the tolerance report on the assembly level. As you stated above there is a drastic difference between the two extremes of your models. Bottom line for me there was no real easy way other than to grind through it by changing the part accuracy and redefining failed features until the model regenerates and then prevent the problem on a go forward basis.

I would advise also to be careful with the "weld features" you mention as in mechanica they are not viewed the same as a conventional weld. The welds in mechanica are used for treating how mechanica extends shell elements during compression. They are not the same as take part A and weld it to part B. That is what the "bonded" interfaces are for. Forgive me if I am misunderstanding your application and sound as if I am telling you what you already know.

Hope that helps and good luck,

- J -

 

[VRUGRU]

Thanks Jvian,

Company-wide change to set the default accuracy to "absolute" might take a while.

However, when I tried to manually change the tolerance of parts to absolute, as I move bottom up, my sub-assemblies (which were meshing fine with the "relative" accuracy), failed to mesh.

I am not using the weld features to create 2-D welds. All the parts are solid models. The "End Weld" feature within Creo is an easy way to extend one part to another, instead of one having to create solid models for butt and groove welds. It creates 3-D solid elements within Mechanica.

 

[brep]

If the system is having trouble merging the parts to create the assembly (due to model accuracy problems), then it is possible to leave a small gap between the problematic parts and then use a rigid link to "join" them. Of course the stresses right at the interface between these two parts could be misleading, but if the areas of interest in the assembly are away from this zone then this would be an acceptable practice. (This method is a throw back to the earlier days of FEA where joining parts using rigid links like RBE3, stiff springs etc etc was the norm)