Using shell elements in Nastran In-CAD

[Anonymous]

Hi there!

Is it correct that Nastran In-CAD can't create midplane mesh of solid parts (like Inventor stress analysis and Simulation Mechanical can) to run an analysis with shell-elements? 

Regards,

Max

[AndrewSears]

Hi Max,

In-CAD will not create a mid-plane from a solid like Inventor stress analysis but that is the only limitation.  Instead we are allowing people to create shells from surfaces.  These can be variable and constant thickness. Right off, I can think of two scenarios.  

First: If you want to use shell elements instead of solid elements then you will need to add the mid-surface manually to the CAD model.  Once this is done you can define a new shell physical property and choose this created mid-surface.

Second: If you have modeled the part using a surface first and then thicken it, you can use that surface as the shell element.  

Both scenarios will ignore the solid geometry as long as you have not given the solid geometry a physical property in In-CAD.

Here is a workflow where the mid-surface already exists.

1) Create the mid-surface.

2) Thicken the surface keeping the surface in the center.

3) Define the shell physical property.  Be sure to select the original surface in the center.  Add a thickness.  If your part has a variable thickness, click the advanced button and add that info.

4) Create the mesh.  If the solid geometry meshes when you have only defined a shell physical property then you selected the outside surfaces of the solid.  Redo the physical property creation for the surface and verify that "Associated Geometry" is checked and your surface shows in the selected field.  The solid will remain visible for now.  

5) Add loads and BC's to the surface edges or faces.  Be sure to not select any of the solid geometry.  

6) Now solve.  The solids are ignored because you did not give them an In-CAD physical property.  You should only see the FEA results for the shell.

  

Hope that helps.  Let us know you have any questions or I should explain something better. 

Andy 

[Anonymous]

Hi Andrew!

Thank your for your answer! The second idea is a pretty good workflow if you know you eventuelly will run a FEA analysis with shell elements.

I guess that if you're starting with a "dead solid" you have to go with first idea. It's primarely this i was interested in, was kinda hopeing that somebody would have a good workflow idea for this, do you have any more suggestions on this? 🙂 Sometimes an assembly has several parts and each part have several surfaces that in turn need to be modelled and well, this could take some time to modell... (Thicken/Offset + Extend + Trim til my eyes bleed)

Are there any plans on haveing a midplane mesh for Nastran (In-CAD)? Couldn't the Inventor midplane mesher be used in some way? I mean, the programming is sorta done, isnt it?

Sorry for the many questions, any reply/idea on anything is very welcome! 🙂

Regards, Max

[AndrewSears]

Max,

You don't need to remodel everything if the solids are done but representing them as a surface for shell elements will take a lot of work, or as you put it, make your eyes bleed.  You will need to create all of the mid-plane surfaces by hand then create a composite surface so you have one single surface. It is not the ideal situation but you can get close if the solid is already created.  The most important part if you go down option 1 is to make sure you create the composite surface from the surfaces and delete the originals.  In-CAD is paying attention to all surfaces and stitching does not remove the surfaces after creating the combined version.  Deleting the originals can be good and bad so do some testing first so you understand the possible issues you will run into.

I am not sure that you should replace sheetmetal (I assumed you were using shells for sheetmetal parts) workflows with with thicken/trim/cut.  You can get creative with sketches and extruding them as surfaces then create the composites.  If you want, send me a part file and I will work through the process showing you how I would use an existing solid model and create the new mid-plane surfaces for shell elements.  If you can post to the forum for everyone else to benefit from that would be great.  If you can't then send to andrew.sears@autodesk.com and I will reply directly with the steps.  

I can't comment on future plans for the product in this forum.  If you want, please post this to the Ideastation.  This way others can vote and we can see how popular this would be with the community.  More votes, more likely to get into the product.  

Andy 

[Anonymous]

Hi Andrew,

I've attached a small assembly of a bridge. Say that i would like to analyze this with shell-elements (disregard that some parts may not be suitable for analysis with shells).

In Inventor stress analysis this is easy, just do a "midsurface" of all parts and they become thinn bodies with all contacts preserved, then you can mesh as shell elements. With Nastran you would have to manually convert the solids to "midsurface" parts in Inventor cad. What would be the fastest way to do this? 

Keep in mind, this is a small problem. Larger assemblys can contain 1-2 thousand parts that one might want as shells.

Regards, Max

[AndrewSears]

Hi Max,

I created a video showing how I would use the solid geometry to idealize specific faces as shells since we do not have an automatic way to convert solids to shells.  The main reason why I selected this method is because it does not require you to modify your production models.  So, grab a cup of coffee and watch this 5 minutes video.  Please let me know if you have any questions.

Thanks,

Andy 

[frederic.levesque]

Hi Andrew!

I am working on a similar model (a welded structure to be modeled with shells), but the offset bonded contact doesn't seem to work. It is set on auto and the offset parameter is slightly higher then plate thicknesses. Hence, similar to what you show in the video. So, I used the same parameters as shown in the video. But, I run into a fatal error everytime, related to contacts. 

FATAL ERROR T2135: UNABLE TO GENERATE SURFACE CONTACT USING SPECIFIED PARAMETERS.

Do you have any idea what could be the problem? 

I am using In-CAD 2016, in case the problem could be related to a bug in the version...

Thank you very much!