Subdividing surface on a solid in FEMAP

[brkica]

Hi,

How can I break a surface on a solid into multiple smaller surfaces? This is necessary in order to enable surface mapping needed for the Hexmesh. Some solids which I import by a step file (usally form CAD) have outer surfaces which have more than 4 edges and can thus not be mapped as mapping requires surfaces of 4 edges.

How can I break the surfaces on the solid, but without breaking the solid in two pieces, as I need just one solid?
Subdivision of surfaces is sometimes also needen in order to apply boundary conditions using the surface.

Regards.

 

[jerzy]

Use the Geometry-Solid-Explode command to separate your solid into surfaces. Modily the surfaces, then use the Geometry-Solid-Stitch command to reform a solid.

Jerzy

 

[jerzy]

"modily" should be "modify"

 

[trainguy]

jerzy,

You seem knowledgeable with FEMAP.

Do you know of any website that has lists of tasks and commands, in the same style as you have written?

The package has so much functionality, its a little bit overwhelming...

thanks,

tg

 

[brkica]

Hi jerzy,

Do you know how to hide components within FEMAP?
(see my other post)

Regards.

 

[brkica]

jerzy,

you can find my other post about hiding components in the Nastran forum.

Regards,

brkica

 

[jerzy]

Trainguy: I agree that FEMAP can be overwhelming. I use the documentation that comes with FEMAP and also search the Web, but have found no one place that completely gives the kind of information that helps get models meshed and solved.
Many of the commands have taken me some experimenting to understand how to use them, and I have a long way to go before I would consider myself half-way knowledgeable about the program. I pick up FEMAP tools when the models I'm working on require me to use them.

brkica: On what Nastran forum can I find the post you refer to? I use the group commands to allow me to work on and view parts of models. Right now I'm working on an assembly of 4 solids. I use Group-set to create a group. Then Group-solid to add a solid to that group. Then group-surfaces to add the surfaces on that solid to that group. I click on the "Method" button on the group-surfaces dialogue box to allow me to select surfaces on the solid I just put into the group. Curves on those surfaces get added in a similar fashion. Once you have defined your groups, View-Select command will allow you to pick a group for viewing.
Once I find the post you referred to, I'll try to answer your specific question.


jerzy

 

[brkica]

Jerzy,

I will try tonight what you just decribed. My post about hiding componenets can be found at:

http://www.eng-tips.com/viewthread.cfm?qid=213676&page=1

But you might have answerred my question alreaady. I will try out tonight.

I agree too that the number of elaborated examples found in FEMAP's documentation is limited. I don't understand why UGS doesn't provide its users with much more example on various type of analysis. Given all the capability of FEMAP they certainly do this, as it is indeed overwhelimg.

Thanks a lot!

 

[jerzy]

Hello brkica,

I found your post: I didn't about the FEMAP forum---I'll have to check it out from time to time.

I use groups rather than layers but I want to experiment with the differences between them to see how best to use them.

jerzy

 

[brkica]

jerzy,

do you know how to break surfaces of components in an assembly? I am trying to break surfaces on one componenent in to smaller surfaces so I can set the mesh size (mesh size on surface) on these surfaces smaller then elsewhere. I want this because one part of the surface to be broken is in contact with another component. How can I set the mesh size near contacts smaller then elsewhere. I quess I need a surface near the contact so I can mesh wvery finely. But how to create this surface? Working with group in order display one of the componenets doesn't work. It displays the solid only, no surfaces. CReating other groups to put in surfaces only does not work either. So, here I need to combine features Explode, Stich and working with groups or layers.

I may post the FEMAP model if necessary.


Regards.

 

[jerzy]

Hello brkica,

I think you have to delete the old surface and create new surfaces to replace the deleted surface.

About groups: the points, curves, and surfaces related to the solid have to be added to the group. I outlined a way to do this one-by-one in my earlier post. In the newest version of FEMAP (9.3.1) there is a command that adds related entities along with the "parent" entity. It is
Group-operations-Add related entities. I create a new group; add a solid to this group; then use the command to add all the surfaces, curves, and points on that solid.
I don't know what version of FEMAP introduced this command.

jerzy

 

[brkica]

Hi jerzy,

I am not able to modify the surfaces of a component from an assembly. When I make the group containing the solid and all its surfaces, curves and points and I explode it, the solid is of course gone but there is no sign of its surfaces, curves and points either. Any idea why?

How can I choose a component from an assembly, make the component visible, explode it, modify its surfaces in the way I want them again again stich the solid so that at the end I have my original assembly with the surface of one of its components modified?

I have no idea!!

 

[jerzy]

Hello brkica,

When you explode the solid, the new surfaces will not be in the original group unless you have selected Group-Operations-Automatic Add before the explosion. The new entities can be viewed if you use View-Select-Groups-None.
You probably had View-Select set to your new group; after explosion the new entities were not in the original group.
Do not be afraid to experiment a little with the different view and group operations: as long as you don't use the delete command, you won't lose your model.

jerzy

 

[trainguy]

Hi brkica.

You should search Femap documentation about boundary surfaces. I don't grasp them 100% (more like 35%), but I think this could help do what you need.

tg

 

[trainguy]

Here are 2 ways to split up surfaces, after using the explode command.

1) Geometry - solid- slice match. Don't be fooled by the fact that this is in the solids sub-menu, because it also works on the Femap surfaces that you have. This provides a straight line cut through whichever "solids" (i.e. surfaces) that you select. You could repeat this several times and if you have too many subdivisions, you could do the reverse operation on a few surfaces by using Geometry Solid Add. Those "solid" commands are totally applicable to surfaces, because they are paraSOLID surfaces!

2) If you don't want a straight line cut, but you need random geometrical shapes, place the workplane on your surface, then do the following:

Geometry - curve (or other shapes you may want) and enter them on your surface.

Geometry - curve from surface - Update surfaces (toggle). This ensures that the next command will actually imprint the geometry onto your surface thereby splitting it up.

Geometry - Curve from surface - Project and select the geometry you just created, then the surface you want to "Burn" it onto.

Cheers.

tg