Showing results for

- Navigation
- Simcenter
- Forums
- Blogs
- Knowledge Bases

- Siemens PLM Community
- Simcenter
- 3D Simulation - Simcenter 3D Forum
- 2D Solid Model

Options

- Subscribe to RSS Feed
- Mark Topic as New
- Mark Topic as Read
- Float this Topic for Current User
- Bookmark
- Subscribe
- Printer Friendly Page

Solved!
Go to solution

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

03-04-2014 09:21 AM

Hello,

I tried for some exercise to set up a simple model consisting of two cylinders in a rigid box and a third cylinder stored on the other two.

As already mentioned, I just want to model a cross section of this in X-Y plane. The problem I have is, that I am not able to mesh the cylinders with CPLSTS or CPLSTN elements. I always get the error message: Some geometry is out-of-plane. These are added to Output Group.

Does anybody have some experience with 2D solid modelling?

Thanks

Georg

Solved! Go to Solution.

7 REPLIES

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

03-05-2014 07:45 AM

Georg,

There's an option in the FEM create/edit dialog that specifies the 2D solid plane. Your options are XY and ZX. It sounds like you have the 2D solid plane option set to none or ZX. NX does do a check to determine if the geometry being meshed is in the appropriate plane. It is seeing your geometry as out of the solid plane. The attached image shows the plane option.

Regards,

Mark

Mark Lamping

Simulation Product Management

Product Engineering Software

Siemens Industry Sector

Siemens Product Lifecycle Management Software Inc.

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

03-05-2014 07:58 AM

Thank you for your answer.

I already checked this possibility, but it is set the correct plane.

I also tried to change the plane to ZX just to see and the result was the same.

When I have a look to the output group mentioned at the error window, all three cylinders are shown as out-of-plane geometry.

Regards,

Georg

Solution

Solution

Accepted by topic author GStrickner

08-26-2015
04:32 AM

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

03-05-2014 08:20 AM

Georg,

Do a Solver Syntax Preview on the mesh and verify that the grid Z coordinates are = 0.0

If there are numerical roundoff issues (i.e. a grid with a Z coordinate of 1.0E-12), you can increase the zero tolerance in the exporter (RMB on Solution, Edit Advanced Solver Options, Formatting, Real Filter) to get 0.0 written out to the input deck.

Regards,

Jim

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

03-05-2014 08:40 AM

thank you for the hint.

I really took care to be inside the plane, but it looks like I made a stupid mistake.

Thank you for your help.

Regards,

Georg

Solution

Solution

Accepted by topic author GStrickner

08-26-2015
04:32 AM

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

03-05-2014 08:49 AM

Georg,

The in/out of plane tolerance check is fairly tight. I encountered this in the past too. My geometry really was out of plane, but only a math program would have picked it up. I got around the problem by using these steps:

1. Generate the mesh as shells. This let me proceed past the error you are getting.

2. Edit the Z coordinates of all my XY plane nodes to be zero. This is possible in the Node Modify Coordinates command.

3. Modify the element type (Modify Type command) of the shells to be plane stress/strain, or axisymmetric

Previewing my shell mesh showed non-zero Z coordinates. After I edited the nodes, the Z coordinates were exactly zero.

Regards,

Mark

Mark Lamping

Simulation Product Management

Product Engineering Software

Siemens Industry Sector

Siemens Product Lifecycle Management Software Inc.

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

03-05-2014 10:04 AM

one additional question I have.

I posted a picture of the model in my first request. There you can see three blue lines that should represent the box.

How can I mesh them in an correct way to be able to apply an edge - to - edge contact between the cylinder and the box?

Regard,

Georg

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

03-05-2014 10:47 AM

Georg,

For SOL 101, 103, 105, 111 and 112, the contact must be defined on element edges. You would have to "thicken" the channel geometry in the plane to make a face that you can mesh with axisym/plane stress/plane strain elements. You can then constran all DOF on the grids associated to these elements of you want them to be rigid.

For SOL 601, you can put a node on the two endpoints and the curve intersections, then use BLSEG to define a target region using the nodes only. The solver will conect the nodes with rigid target segments.

Regards,

Jim

Follow Siemens PLM Software

© 2017 Siemens Product Lifecycle Management Software Inc