January 28, 2018 at 11:42 amFlorisvanelterenSubscriber
I'm working on an analysis that followed from another post that I have made earlier:
Thanks to the solution posted there I was able to model the desired behaviour. However, now I am running into some new problems and I would be greatly helped if someone knew how to handle this. I have attached my model for reference.
I want to model three sheet bodies that are connected by crease lines (crease line modeled with constraint equations). The middle sheet has a bending actuator attached to it. The bending actuator consists of a rubbery matrix material with embedded SMA wires (SMA wires attached to matrix with constraint equations, modeled with orthotropic thermal expansion). I've modeled a quarter of the whole as the setup is symmetrical (it will represent a sort of "sheet body gripper" in the end). In order to get the model to actually fold the crease, a few auxiliary loads were used to "nudge" the model into the right position. In the steps following what I have now, I want to remove all the "nudge"-loads as they should not appear in the analysis, further increase the temperature and apply a load to the tip of the gripper to simulate grabbing something,as shown in the illustration. In the end I want to analyse the force-deflection behaviour of the tip.
When trying to remove one of the nudge loads and further increasing the temperature, the analysis is not able to converge no matter how small I make the substeps. I've attached the unconverged model to this post. It seems some elements start to warp a lot as shown in the screenshot below (the matrix element in the middle is starting to warp). I can't figure out why the analysis does not continue. So my question is if anyone has an idea to make this analysis more robust?
Thanks in advance!
January 28, 2018 at 12:56 pmpeteroznewmanSubscriber
Your attachment only has the v17a.wbpj file and not the v17a_files folder that is required to open a project. You need to put the folder in the zip file as well.
Alternatively, in Workbench, you can use File, Archive... to create a v17a.wbpz file that does this operation for you, and I would use File, Restore Archive to unzip it. You can use the Attach button to upload a .wbpz file.
What version of ANSYS are you using, 17.2 or 18.2?
January 28, 2018 at 1:11 pmFlorisvanelterenSubscriber
Ah right! I've now edited the post to include the .wbpz file (240 MB), I think it's quite a large file so uploading takes a while (I should have been aware that a 250 kb file probably wouldn't cut it!). I am using version 18.1!
January 28, 2018 at 1:24 pmpeteroznewmanSubscriber
Should have mentioned that there is a 120 MB file size limit.
To reduce the size of the .wbpz file, in Workbench, right click on Model and Clear Generated Data (or in Workbench, do that on Mesh), then save the file and create the Archive.
January 28, 2018 at 1:42 pmFlorisvanelterenSubscriber
Thanks! Yess, that helped, I've now included the smaller .wbpz file.
January 28, 2018 at 1:44 pmpeteroznewmanSubscriber
You are lucky I still have 18.1 on my computer. If I only had 18.2 you would not be able to open any file I edited. I successfully opened the archive and will take a look at it today.
January 29, 2018 at 4:13 ampeteroznewmanSubscriber
Material and Element Changes to Control Hourglass Mode
The elements around the wire end were beginning to "hourglass". I added two methods to help control that as described here, which require a command snippet to turn on two Keyops in the elements and to add a Hyperelastic material model to the Matrix material.
I sliced the substrate so there was an edge that matched the matrix. I did a merge on the edges along the curve on the substrate.
I used two elements through the thickness of the thick matrix solid, doubled the mesh densitiy along one axis of the matrix, and biased the mesh density along the other axis of the matrix.
You had contact between the thin and thick parts of the matrix. I deleted that since the two solids were already sharing topology in a multibody part in DM.
Changes in v17d
In your model, you had a large set of constraint equations connecting the SMA wires to the matrix. I replaced that with contact. Maybe that is the same. The large number of contact elements between the substrate and the matrix prevents the model from scaling the solution time as more cores are added. Unfortunately, v17d will not run to completion, it stalls at 4.7.
Changes in v17e
I deleted all the contact and constraint equation for the SMA wires and used the Mesh Edit to merge coincident nodes. Now the solution time scales well as more cores are added. I suppressed the Moment Nudge, and reduced the Force nudge to 0 at step 4, which is also the final step. You may like this model better, it certainly solves much faster (138 seconds on 16 cores ANSYS 18.2).
Look at the puckering where the SMA wires are pulling the matrix.
The attached archives are in ANSYS 18.1 format.
Another question is whether the Matrix material should have a higher Poisson's Ratio. Most elastomers have values higher than 0.45, yours is at 0.3.
January 29, 2018 at 8:37 amFlorisvanelterenSubscriber
Thanks a bunch! I was obviously missing some knowledge on the different options that I had to make mesh connections, solve hourglass problems etc, so this has been super helpful already. I took a look at your new model yesterday already and the physics are more realistic as you have stated before. I'll check out the newest version in a minute.
Regarding the poisson's ratio: I'll change that asap to a more realistic value, it was something that I hadn't adressed yet, I have read your post on the hyperelastic model so I can sort that out myself.
Once again, thanks a lot!
January 29, 2018 at 12:24 pmpeteroznewmanSubscriber
You're welcome, it's an interesting project. I liked how you used the CEINTF command to create the hinge.
January 29, 2018 at 6:32 pm
- You must be logged in to reply to this topic.
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.
- Saving & sharing of Working project files in .wbpz format
- An Unknown error occurred during solution. Check the Solver Output…..
- Understanding Force Convergence Solution Output
- Solver Pivot Warning in Beam Element Model
- Colors and Mesh Display
- How to calculate the residual stress on a coating by Vickers indentation?
- whether have the difference between using contact and target bodies
- What is the difference between bonded contact region and fixed joint
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- User manual
© 2023 Copyright ANSYS, Inc. All rights reserved.