March 6, 2017 at 6:49 pmmingyao.dingAnsys Employee
I would like to get the shape/geometry of the result of a structural simulation I ran.
October 22, 2017 at 4:11 pmpeteroznewmanSubscriber
There are two approaches to get the deformed geometry out of a Static Structural solution into a CAD program: a two step process and a fifteen step process. Thanks to SimuTech group for teaching me this method.
FOR VIEWING OUTSIDE FACES ONLY
In Mechanical: Insert a total displacement for a selected body into the solution, then right click on it and export an stl file.
In CAD: import the stl file. Some CAD systems don't handle imported stl files very well. New versions are getting better at that. See the next approach.
TO CREATE A SOLID BODY (more useful in CAD programs)
Here are the steps to export a Parasolid file:
- Create a Named Selection named "top" that contains the part you want to export.
- Analysis Settings set to Save APDL db
- Drop a Mechanical APDL component onto the Static Structural Solution
- Right click on Analysis row of Mechanical APDL system on project page and select "Add Input File"
- Select attached input file upgeom.inp (this is setup to select a single part in your model).
- Drop an FE Modeler component onto the Mechanical APDL Analysis
- Update the Static structural solution, Mechanical APDL Analysis, and FE modeler.
If the Static structural solution was done before step 1 above, clear generated data first.
Open FE Modeler
8. Right click on "Geometry Synthesis" and select "Insert>>Initial Geometry"
9. Right click on "Initial Geometry" and select "convert to parasolid"
10. Drop a DesignModeler (Geometry) Component onto FE modeler Model cell
11. Update FE modeler and DM
Start DM (double click on Geometry field)
- Add a Body Operation, "Type" set to Sew, setting the "Create Solids?" to Yes
If the result is not a single solid, change "Tolerance" to User Defined.
13. In DM open Tools>>Options then go to:
DesignModeler>>Geometry>>Export Options>>Parasolid Export Version and select 24.0 for NX8
14. Export Parasolid file.
15. In CAD system import Parasolid file.
October 22, 2017 at 4:40 pmpeteroznewmanSubscriber
This site won't allow a file with an inp extension to be attached, so below is the contents of upgeom.inp which is attached as upgeom.txt
October 31, 2017 at 11:35 ampeteroznewmanSubscriber
Does AIM have a method to get the deformed geometry back to SpaceClaim?
May 22, 2018 at 9:42 amCakeOrDeathSubscriber
Great walkthrough! However, I seem to experience a problem when converting to a parasolid. Even though my initial geometry turns out OK, all faces, vertices, etc are detected correctly, when I convert to parasolid it doesn't detect any of the geometry correctly. I'm just trying the process out with a deformed beam so I wouldn't have thought it was too complicated to handle.
May 22, 2018 at 9:58 ampeteroznewmanSubscriber
Please attach your workbench archive .wpbz file and let's take a look. Also say what version of ANSYS you are using.
You would think ANSYS would build-in a useful output in a simple way, such as right mouse click > Export Deformed Geometry.
May 22, 2018 at 10:19 amCakeOrDeathSubscriber
Thanks very much! Hopefully I have created the .wpbz file correctly, but if there are any issues then please let me know.
I'm using ANSYS version 17.1.
Indeed! Clearly there is a need for people to use the deformed geometries in CAD software or for further analysis in other software packages, so you think it would an easier process.
May 23, 2018 at 2:52 pm
May 24, 2018 at 10:47 am
January 8, 2019 at 2:03 amearvinlloydSubscriber
Now that FE-modeler is phased out (in 19.1 and newer), what is the substituting procedure (besides exporting to .stl)?
January 8, 2019 at 10:19 amRobAnsys Employee
It's been relabelled as "External Model", so try that.
April 11, 2019 at 9:17 amlordofthethingsSubscriber
Both External Model and Mechanical Model are not attaching with Mechanical APDL.
May 31, 2019 at 1:43 pmNRafaelSubscriber
I've been trying the procedure to obtain the solid model. But I am not understanding the step 5. Where I am supposed to get that input file?
June 9, 2019 at 12:35 pmpeteroznewmanSubscriber
This post has the text for the input file. Just rename it with a .inp file extension.
October 11, 2019 at 8:04 amlincs2k9Subscriber
As "FE modeller" is not available in Ansys latest version, this thread's procedure is not applicable for latest version ansys workbench. "External Model and Mechanical Model" are not working according to this procedure. Can you provide instruction using latest version? Is it possible?
October 21, 2019 at 4:53 ammehdimechanicSubscriber
Can this single part in step 5 be an assembled part? some parts together? then how should the input be modified?
November 5, 2019 at 11:39 amlordofthethingsSubscriber
For newer versions of Ansys that do not have a "Finite Element Modeler"
1. Run the simulation to get deformed geometry :
2. Connect the solution part of the static structural to a new instance of "Mechanical Model", update the tolerance if necessary, and check the following options in the properties of the Mechanical Model. Update both the systems.
3. Finally, bring a new instance of the "Geometry" system and connect the model to it.
4. Open the Geometry module in DM (Not Spaceclaim), generate it, and then File --> Export --> (STEP format). Wait until the conversion is over. Now you have the solid model ready!
November 13, 2019 at 11:44 amRobAnsys Employee
Have you also linked Engineering Data?
Edit: don't need that, and it works fine here.
November 14, 2019 at 3:05 pmlordofthethingsSubscriber
Instead of dragging the mechanical model on top of the static structural, drag and drop it first as a stand-alone module BESIDE static structural (dont link it yet) Once you are done, take the solution cell from the static structural and join it with the mechanical model's Model. This should then work.
November 27, 2019 at 1:11 amrajansanandSubscriberBut...how to provide a fixed amount of imperfection (my model has to be given a fixed amount of imperfection by multiplying a value to the deflected shape i got in eigen value buckling analysis)
November 27, 2019 at 11:07 ampeteroznewmanSubscriber
rajansanand, this discussion is about how to convert a deformed mesh into geometry.
You are asking a different question, how to deform a mesh to use as the imperfection for a buckling analysis.
Please open a New Discussion for this question, or do a search on the site to look for an answer.
March 25, 2020 at 2:01 amnabilkhalid56Subscriber
I am trying the same method but the geometry I get in the Mechanical model isnt as deformed as it is in the solution of Static Structural. My properties settings in the workbench for the Mechanical model instance is similar to what is described in "lordofthethings posted this 05 November 2019". Can someone please help? I have also attached the image.
March 25, 2020 at 11:18 am
March 26, 2020 at 6:37 amnabilkhalid56Subscriber
Yes, the scaling of the results was the issue. Thank you so much for your fast response.
January 26, 2021 at 8:50 pmSnow1RunnerSubscriberHi everyone, nFor the process outlined by where does one can modify the tolerance. I've got a very small deflection in a plate and when I complete all of the steps, I can't appreciate any deformation. nI can see the deformation in DM before exporting the STEP file so I am pretty sure it's not the same case as the one above of the scaling of the solution. nRegards! n
January 28, 2021 at 6:01 am
February 24, 2021 at 9:21 pm
March 13, 2021 at 12:31 amsbalasubramanyamSubscriberHello!nnI'm trying to export the deformed geometry from my Static Structural analysis, to be able to use the deformed model in HFSS simulation. The model I'm using is an assembly consisting of few components. nI'm using ANSYS 2020 R2 and tried following the steps provided in this discussion. For some reason, when I try to open the deformed geometry, it opens in Space Claim instead of Design Modeler. This is even after changing the settings to modify models in Design Modeler.nReally appreciate any inputs!!n
- You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- Solver Pivot Warning in Beam Element Model
- Saving & sharing of Working project files in .wbpz format
- Understanding Force Convergence Solution Output
- An Unknown error occurred during solution. Check the Solver Output…..
- What is the difference between bonded contact region and fixed joint
- User manual
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- whether have the difference between using contact and target bodies
- material damping and modal analysis
- Colors and Mesh Display
© 2023 Copyright ANSYS, Inc. All rights reserved.