Removing features of an assembly for simulation in ANSYS

[JONOLN]

Hi!

Is there an elegant way of removing details and features from an assembly without getting a pile of regeneration failures?

I am fairly new to Creo, and I'm stuggling with preparing large assemblies for simulation in ANSYS. The assemblies I'm working with contain lots of details that are not of interest in for instance a modal analysis, for instance holes and rounds, and they add unnecessary complexity to my model. If I try to suppress these details, I end up with a long list of regeneration failures, which often lead to the assembly not being imported correctly into Ansys. Going through the list and updating placements and references is extremely tedious.

Ideally, I'd like to remove all references so that the parts are independent and changing one part won't affect any other part. Is this, or something similar, possible?

[tbraxton · Accepted solution]

Short answer is no. The parent child relationships are a result of how the models were created. There are options to manage this inside of Creo if you do not have the ability to debug the models when suppressing features.

I would first ask the designer(s) of the parts to submit models suitable for simulation. I have always required my design teams to support the simulation teams by providing geometry suitable for meshing and SIM. We will construct beam, shell, midplane, CFD volumes etc., basically whatever was needed for simulation. Of course we want to know before designing the CAD models what simulations will be using the geometry to plan for it when building the models.

Assuming the models are "spaghetti code" in their construction then I would try one or more of the following. If the models have many assembly features created in individual parts that is not generally considered best practice and this will be extra painful to manage.

Try managing the feature suppression in part mode, not in assembly mode.

If after suppressing the features in a part yields the geometry you want for SIM then set all of the features to read only and you will not have regen failures with this part while set to read only.

model->operations->read only

For each part in the assembly of interest.

Save the part as a Creo neutral file. This will create a "dumb" import geometry without features in the tree. Open the neutral file version of the part and then use the flexible modeling functions to defeature it. Flexible modeling is similar to Ansys Spaceclaim and can quickly de feature many models, particularly if they are primarily built of prismatic shapes. it has the ability to remove rounds/chamfers etc.

[JONOLN]

Thanks! I will try out your suggestions!

[KenFarley]

Whenever I do structural analysis I generally end up creating parts and assemblies specifically for the analysis. I always have to simplify the part (remove holes, small rounds, etc.) or parts. Otherwise, meshing will either take an extremely long time, or fail completely. Even if the model as designed is able to be meshed, the analysis will often be too much for my system to handle.

If it's me doing the modeling, and I know I'm going to be analyzing the device, I can build the models with a "simplified" version in mind, but that's not usually the case.