turn on suggestions

Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.

Showing results for

- Navigation
- Simcenter
- Forums
- Blogs
- Knowledge Bases

- Siemens PLM Community
- Simcenter
- 3D Simulation - Femap Forum
- Coordinate transformation using plain strain eleme...

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

11-18-2016 03:58 AM - edited 11-18-2016 04:00 AM

Dear all,

The application of coordinate transformation works well for 3d continuum elements, but not for 2D plain strain elements. I prepared a simple example for testing. Have a look to a simple beam with the dimensions height = 10 mm, length = 100 mm, width = 100 mm (thickness of plain strain) constrained on the left side and a tensile load on the right side.

Creation of 2D plain strain elements with mid nodes (CPLSTN8)

Solution based on global coordinate system (sigma_xx = 100 MPa):

Next I want to transform the stress results to the local coordinate system (see bottom right edge in above figure).

**1) First attempt over Select PostProcessing Data and Transform**

leads to the following errors:

Transverse results exist and are ignored in transformation

Transformation of vector 7220 can not occur as vector 7223 does not exist

Transverse results exist and are ignored in transformation

Transformation of vector 100420 can not occur as vector 100423 does not exist

Transverse results exist and are ignored in transformation

Transformation of vector 150420 can not occur as vector 150423 does not exist

Transverse results exist and are ignored in transformation

Transformation of vector 200420 can not occur as vector 200423 does not exist

Transverse results exist and are ignored in transformation

Transformation of vector 250420 can not occur as vector 250423 does not exist

That’s clear, because plain strain isn’t a plate or laminate stress. The option for solid stresses and strains also doesn’t work.

**2) Second attempt over Model->Output->Transform**

leads to the same behaviour.

**3) Last attempt over nodal stresses** (Model->Output->Process-Convert average) and transform Nodal Vector Output (first option in above figure) also doesn’t solve the transformation problem, because the nodel stresses doesn’t appear in the “Select Output Transform”-dialog box.

Are there any suggestions to solve coordinate system transformation using 2D plain strain elements?

Many thanks in advance.

Best regards

MaPi

Solved! Go to Solution.

3 REPLIES

Solution

Solution

Accepted by topic author MaPi

11-28-2016
07:01 AM

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

11-22-2016 05:06 PM

MaPi,

Thanks for your post. We currently don't support coordinate transformations for plane strain elements when they're written as CPLSTN* elements - it is something being considered for future enhancement though. Unfortuantely we didn't explain this properly via the error messages that are written out, so my apologies if they were confusing or misleading.

Depending on your needs, there is a potential workaround you can try - by default when you create plane strain elements in FEMAP, we write out PSHELL/CQUAD*/CTRIA* elements instead of PPLANE/CPLSTN* (the latter is chosen by changing the default formulation for the shell elements in FEMAP). In order to get PSHELLs to behave as plane strain elements, the MID2 value is set to -1 which, per the QRG,

For plane strain analysis, set MID2=-1 and set MID1 to reference a MAT1

entry. In-plane loads applied to plane strain elements are interpreted as

line-loads with a value equal to the load divided by the thickness. Thus, if a

thickness of “1.0” is used, the value of the line-load equals the load value.

Pressure can be approximated with multiple line loads where the pressure

value equals the line-load divided by the length between the loads.

This should accomplish the same thing, and we do support transformations for PSHELL elements. Keep in mind, however, that it is treated as a 2d tensor, so the only valid transform is going to be one in plane with the element, even though our 2d tensor transforms are planar projections. Additionally, PSHELL elements don't recover a sigma Z, so if you're concerned about that quantity, you'll need to also run as CPLSTRN* and combine the results.

Finally, the thickness property is ignored on the PPLANE card for CPLSTRN* elements, while thickness is not ignored for PSHELL - for linear analyses, the stress is ratioed accordingly.

With regards to your final point about not being able to transform converted results - that will hold true for any result vectors in the 9mm range - the basis isn't preserved once the conversion is done, so transforms need to happen before data conversion.

Hope that helps.

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

11-28-2016 04:59 AM

big thx for your answer. Dealing with 2D elements like plane stress and plane strain is a little bit confusing in Femap. Coordinate transformations will work only in 2D plane, thats clear. In future, is it possible to merge both plain strain formalism (default and CPLSTRN...) to one, to handle coordinate transformations and Sigma_z together?

Nevertheless your workaround is functional, but complicated.

Best regards

MaPi

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

11-28-2016 11:07 AM

MaPi wrote:

In future, is it possible to merge both plain strain formalism (default and CPLSTRN...) to one, to handle coordinate transformations and Sigma_z together?

Unfortunately not, because this is a Nastran limitation. Remember that the default plane strane formulation uses PSHELL where MID2=-1. Even with the plane strain option enabled, PSHELL elements do not return a sigma Z, whereas CPLSTRN elements do. This requires two separate runs.

We will look into adding transform functionality for CPLSTRN based on your request though, and this should help make things more straightforward in the future.

Follow Siemens PLM Software

© 2017 Siemens Product Lifecycle Management Software Inc