April 25, 2018 at 2:34 amtrayCSubscriber
Hi I am trying to mimic fetal head deformation after passing through the canal and was wondering if anyone had any tips to help my results converge?
I modelled the suture material as a mooney rivlin hyperelastic and the cranial bone as linear elastic. I am unable to attach the file because it is so large.
this is the onedrive link: https://1drv.ms/u/s!AvOVvBGcNU10hVSj0x9Ncgv2iEvb
I modelled the suture material as a mooney rivlin hyperelastic and the cranial bone as linear elastic. I cant attach my file because it is too big.
These are my contact setting between the bones(dark yellow and grey) and sutures(light grey)
the contact between the vaginal canal and fetal skull was made as frictionless
I placed a displacement of the fetal head of 100mm in the y direction, through the vaginal canal (which is a fixed support)
April 25, 2018 at 5:53 ampeteroznewmanSubscriber
Hi Tracey, nice detail on the head!
Contact is best defined between faces. Your model has 4 bodies contacting a face, which will work but may create more equations to solve than you need to resolve the contact between the faces.
Both the inner and outer faces of the vaginal canal are selected for Fixed Support which means those faces can't move at all. You don't want that. In your previous post, only the outer face was fixed.
You have applied a displacement in a cylindrical csys to every outer face on the head of zero displacement in the tangential direction. That is going to prevent the head from deforming "naturally". If the contact forces were to push in such a way that some area of the head wanted to move in that direction, but not other another area, the displacement boundary condition would prevent that deformation. You don't want that.
Displacement 2 is not what you want. It requires that every node on the outer surface of the head moves the exact same y distance in time.
Have you ever seen a peeled hard boiled egg sucked into a bottle? You can see how as it squeezes its way through the neck, the egg elongates. That kind of motion is prevented by Displacement 2.
The above explanations help to explain what not to do and why your model may not be converging, I will make another post when I have a better idea on what to do.
Is the geometry 1000 times larger because you wanted to try to solve this in Explicit Dynamics? You have used a Transient Dynamics system that gets no benefit from the scaled geometry, but it is convenient if you want to try Explicit Dynamics.
April 25, 2018 at 6:24 amtrayCSubscriber
Thank you for pointing those things out!
The model is 1000 times larger because I modelled the fetal head based on a 3D scan and the dimensions were 1000 times bigger. When I tried to scale down the model in Solidworks it turned my solid model into surfaces, so I decided just to have an extremely large model.
April 25, 2018 at 6:27 amtrayCSubscriber
I applied a 0 displacement in a cylindrical axis on the fetal head in the y-direction because previously the fetal head would spin a lot when passing through the vaginal canal and I did not want this rotation.
April 25, 2018 at 6:42 ampeteroznewmanSubscriber
Add friction and the spinning head should go away.
April 25, 2018 at 6:58 ampeteroznewmanSubscriber
Another thought is that a head is filled with a lot of fluid, and fluid is nearly incompressible. It's a bit like a water balloon, when you squeeze the diameter, the internal pressure causes the ends to bulge out. You have modeled an empty head, so when the sides are squeezed, they will just push in without any internal pressure that would bulge the top and contribute to "cone head".
After you get your empty head working, you can fill the head with fluid to see the effect.
April 25, 2018 at 11:21 amtrayCSubscriber
yes, that is a good point. I am planning on also adding another material on the inside that resembles brain matter
April 26, 2018 at 3:46 ampeteroznewmanSubscriber
Here is what I would try to get the next version working.
Change your system to a Static Structural model.
Cut a face into the base of the skull where the spine would be. Use that face to push the head along the y axis.
Hold the flat face at the uterus end of the vagina with a displacement BC in the cylindrical coordinate system and set Z and Y to zero, while leaving X (radial) free.
You might have to turn on Weak Springs in Analysis Settings so the solver doesn't complain about parts not being fixed.
Put all the head parts into one multibody part so you can suppress the contact holding them together which will reduce solve time.
Use a Sweep mesh control on the vagina, sweeping radially, so you can assign two elements through the thickness.
The archive is too large to attach, so here is a link to it on Google drive. It won't mesh, but I will fix that tomorrow.
April 27, 2018 at 5:14 pmpeteroznewmanSubscriber
The head may look nice, but it hides a complex history of its journey from CT volume to solid model, and unfortunately, that history is sometimes revealed during meshing or some geometry operration. I would like open a new discussion on the difficulty of converting CT volumes to solid models suitable for meshing in ANSYS because it is very difficult. I would be interested to learn the details of the process you went through to get that SOLIDWORKS file from the original CT volume. I have been studying that process with maurya, here is one discussion.
What I did to avoid the complex geometry is create new head geometry from scratch using the NX11 realize shape feature that allows me to pull faces like putty until I get close to what I want. I did this quickly so I could show you a working model. If I took more time, I would superimpose your head geometry as I pulled on the new body to get them to match closely. I didn't take the time to slice the head up into representative plates, but I changed material on a few surface bodies on the top of the head.
I extracted the faces of this head and created shell elements that were assigned the 3 mm (or in this case the 3 m) thickness. The head was created using symmetry, so I cut the model in half on the symmetry plane.
The video above has an element size half that of the attached ANSYS 18.2 archive. I had to reduce the mesh size to get it to run on the Student license since contact elements are counted as well as nodes and elements in the visible mesh. The attached model runs in about 19 minutes on my 2-core laptop.
April 29, 2018 at 8:35 amtrayCSubscriber
Hi, thanks for your help
I actually used a 3D scanner to scan a fetal skull and imported this as an STL file into SolidWorks. Opened the file as a graphics and just created sketches based on the fetal head shape and lastly used loft and boundary boss/base command to create a solid.
April 29, 2018 at 8:36 amtrayCSubscriber
is it possible to import geometry file from ANSYS 18.2 into 18.1 ?
I only have a research license for ANSYS 18.1
April 29, 2018 at 3:40 pmpeteroznewmanSubscriber
Attached is a zip file of the Parasolid geometry that I imported into DesignModeler to make the video above. I can remake the model in 18.1 if you like.
I can also send you a regular sized version of this geometry, since I scaled it in SpaceClaim after I shaped it in NX11.
When you say 3D scanner, do you mean an optical laser scanner that was just scanning the bone surface? I would be interested to get a copy of the STL file that came from the 3D scanner if you can share that.
April 29, 2018 at 4:15 pmmauryaSubscriber
Can you make a video of convertion of stl graphic file into 3D model.
your model is looking more better i tried in solidwork with vertebrae but its having patches creating difficulty in meshing.
If you are are using window 10 than press and hold window key and press G : game video recorder will open : you can record it.
May 3, 2018 at 11:39 amtrayCSubscriber
Hi i have attached the fetal head scan. I used 3d scan master plus which utilises a structured lighting, so yes it was just the bone surface.
thank you for the parasolid file
May 3, 2018 at 12:00 pmpeteroznewmanSubscriber
Attachments are limited to 120 MB file size. File extensions allowed include .zip and .wbpz among others.
May 3, 2018 at 1:21 pmtrayCSubscriber
Hi Maurya, sorry i do not have time to make a video on how i created the model but i can detail the steps i took. I was unable to directly convert the scanned stl file into a solid part that was usable in ANSYS so instead i used the STL as a guide to create a similar skull model
1. open stl as graphics file in solidworks
2. based on graphics file created sketches along the skull
3. used loft boss to create solid geometry
4. used filled surface to create the ends of the geometry
5. used knit surfaces and ticked try create solid in the settings to convert the surface into a solid
You could similarly use loft boss to create the geometry of the spine but it only be a simplified version
May 3, 2018 at 6:42 pmmauryaSubscriber
i will try this.
May 4, 2018 at 12:40 amtrayCSubscriber
link to fetal head scan
May 4, 2018 at 11:10 ampeteroznewmanSubscriber
Thank you trayC!
- 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.