I am performing a Static Structural loading test but I am unable to enable self contact so that the body elements will not pass through each other.
I've checked the tutorials and found the 'self contact: yes/no' option is only present in Explicit Dynamics analyses involving 2 or more bodies. I have only one body.
Is anyone able to point me to the option to turn self contact on?
defining self contact in static structural
- 242 Views
- Last Post 2 weeks ago
Please post a picture showing the underformed shape of the part, and the shape of the part when it is highly deformed.
The solution is to break the body into separate surfaces and define a frictional contact between those surfaces. See this post and the few that come after it, especially the video!
but the number of surfaces in our model is about 70 .defining 70 frictional or frictionless contact will increase the run time and the run will be impossible.the model pictures is not exist in this pc that that i write this answer,but the model is a honey comb 3d structure where loaded in lateral sides.and the strain is about 50%.Because the energy absorption is the aim of this simulation.i apply displacement and force,but non of this boundry conditions is useful for governing a solution with defining 70 contacts.
please show me another way for this problem.thank you
Complex simulations take a lot of computing time, that is why engineers are constantly looking to idealize the system and solve a simpler model. I have done simulations of a honeycomb sandwich, but I didn't need to go past the elastic range, so an orthotropic material model of the core was all I needed to apply to a continuum solid model. In your case, you need a fully detailed model. The best you can do to minimize the solve time is to have a machine with enough RAM so the solve is performed in-core and not out-of-core. If you have a computer with many processors, like 8 cores or more, then you can use parallel solving to reduce the wait time. I assume you have taken advantage of symmetry if it exists.
Workbench has excellent face selection tools that make it possible to pick 30 faces in a single operation and put those in a Named Selection to go on one side of the contact definition, and pick the other 30 faces to put in another Named Selection to go on the other side of the contact definition. Then define just one of the contacts and use the Object Generator to make the other 29 contacts. In that video you can see 20 faces being selected by one click.
If you want help with that, you can attach a Workbench Project Archive and I will see if there is a way to quickly create the contacts.
Another approach is to move the model over to Explicit Dynamics where body self contact is built into the solver. However, you will find the solve times there will be even longer than in the Static Structural solver and you will have to try to get it to provide a quasi-static solution, which is not easy.
As I understand from your answer,Explicit Dynamics is not an appropriate approach for solving this simulation.
But for static structural,if I define a frictional or frictionless contact that both of contact and target[contact:1 body,target:same body],is an appropriate approach for solving or isn't?and computing time will be change?
Explicit Dynamics is the last resort when all attempts to converge in Static Structural have failed. The reason is that Static Structural depends on finding equilibrium at each increment of load by moving nodes around and sometimes it fails to find that in complex contact conditions. Explicit Dynamics doesn't move nodes around to find equilibrium, it just moves them according to simple physics because it takes such tiny time steps, that it is always in equilibrium.
In Static Structural, you will define contact between faces. It doesn't matter if the faces are on the same body, but they have to be different faces. If you expect self contact on the same face, it is a simple matter to divide the face in the geometry editor so you get two faces and can select one as the target and the other as the contact side of the pair.
You don't even have to have separate faces if you set the behavior to Symmetric. That covers the face with both Contact and Target elements so it can detect self contact. That is a bit more computationally expensive than having separate faces, but if it is a lot of work to get separate faces in the geometry, it might be worth it.
Whenever you add contact to a model, it becomes much more challenging to guide the solver to convergence of the full load. There are many controls to ramp the load in small increments so that convergence develops along the way. It is these extra iterations inverting the matrix that increase the computing time. There are ways to be efficient and take large increments of load when you can, and only use small increments of load when it is needed to minimize the total time. The best tool to use to observe the efficiency of the process is to click on Solution Information and select the Force Convergence plot in the Solution Output. When convergence fails, then you need to look at the Newton-Raphson Force Residual plot to see where the problem was.
I can help with those problems when they arise.
my idea was defining one contact instead of defining several contacts that target and contact elements were whole of the body(contact and target elements can be define for body instead of face or surface)what is your idea about this? is this approach true and reliable?
I have always used face contacts and never body contacts. I think body contacts just put contact elements on every face. This might be a good shortcut for your model. The contact elements are reliable and are the same however you create them.
Can you post a picture of your geometry?
I will provide appropriate pictures from my model and contacts as soon as possible.Thanks for your attention .
I am uploading picture of my model.for simulating compression test in universal test machine,I define two rigid plates in the top and bottom of model in z-x plane and apply two remote displacements in rigid plates.bottom plate was fixed completely and top plane is moving in y direction.Two frictional contacts is necessary between rigid plates and the body. Between surfaces of each cell contact will occurred because the strain is 50%.
I have seen this cell structure before. It is to make an Auxetic material, which has a negative Poisson's ratio. Can you share the geometry with me? If so, please attach the geometry file or make a Workbench Project archive. Have you tried making a shell model of this? What about a 2D plane strain model?
As you say,this model is Re-entrant model that has negative Poisson's ratio and because of this feature ,under compression,body surfaces will touch each other.I am uploading the 3d geometry file.
About 2d plane strain modeling,as I know,this assumption is not true for this model.because the model's length in z direction is not enough long.But shell modeling,maybe good idea for decreasing run time.however the results maybe change a little.3d geometry file
Sorry,I have not workbench project archive in this pc .it;s OK?
Go it. Attached is the sheet body version in a zip file.
But the attached file is not one body and needs to combination of surfaces.I coudn't combine them.Can you tell me how you create this model from my model?
You mesh (I added Face Meshing control) then use a Mesh Edit to merge nodes that are within a tolerance value.
That will give you a connected mesh.
If you have a material model to share, please attach the xml export in a zip file attached to your reply.
About material,the ABS polymer is the material.In one of my references material property of this polymer is discussed only in the elastic region,but i think maybe plastic region also is necessary.Perhaps because of little rupture strain of ABS ,the authors of that reference decided to give ABS a brittle materialthis table is from that reference
I made a quick test model to try out contact and added four contact pairs to pick up the first four contacts that are made.
My model is different from what you want. I made fixed supports of all the ribs on the bottom and brought all the top ribs down by 10 mm in Y while holding X and Z fixed at 0. However, it allowed me to test the contact, which worked quite well.
Attached is an ANSYS 19.1 archive.
I am so grateful for your attention and pursuit.
the contact problem was solved by defining true shell thickness direction(bottom or top) and I have prepare an archive by ANSYS19.0 that share to you.Please tell me the objections of this file .I define all of contacts and aplly remote displacement for rigid plates.Although shell modeling decreases run time,but the run time is about 3 hours and with errors.I think by increasing the number of initial and minimum sub steps, problem can be solve.If you have a better idea,tell me please.
Best https://ufile.io/tvw95 regards
And I defined the pinball region for all of the contacts program controlled.It seems that for some of the contacts I should define big radios for pinbal region such as 2 mm .Do you agree with this statement?
And how you create shell model from my solid model?Are you create that from zero point or there is another way for changing solid to shell?
Excuse me if I ask many questions.I am so thankful and grateful and I wish the best for you
I ran your model to the point where it did three bisections in a row, which is when I stopped the solver.
Before I ran the solver, I set the Newton-Raphson Residuals to 5.
That let me plot the N-R residual force on the elements to see where it had the maximum value. I see the max value on the elements near the edge that has three panels meeting.
I think the corrective action is to make smaller elements near that edge on all three panels if you want the solution to make further progress.
However, if you plot the Equivalent Strain, it solved to a strain of 30%, and we know that material fails in a tensile test at about 25%.
Continuing the simulation further using only linear elastic material properties is just creating false information. If you want to continue crushing the block, you need to introduce a plasticity model for ABS. What is your simulation goal?
I should say that there are different ABS polymers in the market that have different properties.I searched in net and found that the elongation at break of ABS is 3-75%. I searched my material's property and find this file that is exactly my material.ABS plus-P430
As I highlighted in the file the elongations at break and yield are 6% , 2%. with a simplifier assumption we can get the linear elastic and linear plastic region for this material.
My simulation goal is calculating energy absorption of this structure.And that is why the strain is about50% and I defined force reaction probe in my model archive.By plotting force-strain curve from software and changing it to stress-strain curve the total energy absorption of structure will be calculate.
I'm guessing that you are 3D printing this structure. Here is a paper studying the tensile strength of ABS P430 material when printed in a 3D printer. There is a large difference in elongation at break depending on the direction of stress relative to the direction the material was printed in.
Below is the directions in which the test samples were printed, and the tensile stress was applied along the length of those test samples.
Here is Figure 4 from that paper.
What you can see from the plot above is that the point of fracture for material with tension along the Z axis of printing is at a strain of about 1.5% but the point of fracture for material with tension along the 90-deg XY direction is over 8% strain.
I assume you are printing your structure layer by layer with the Z direction up, and will therefore avoid stress in the weakest Z direction. But that still leaves the material elongation varying between about 3 to 8 % total strain.
It does look like a simple Bilinear Kinematic Hardening Plasticity model with a zero Tangent Modulus will take that material past yield. But all the above data is not for the ABS Plus.
I found a thesis that had ABS Plus P430 and that showed a yield strength significantly higher than the 10 MPa shown above. Here is the tensile stress strain curve from that thesis.
Again, ignoring stress in the z direction, the yield in the x direction is over 30 MPa at room temperature, which is consistent with the data you found. This graph shows strain up to 4%, but it doesn't seem to show the point of fracture, which is a critical value to determine when a simulation model goes from simulating reality to going past the point of fracture and starting to create false information. Let's assume that 6% from your reference is the Total Strain at which fracture will occur.
When you say you want to simulate 50% strain, you mean that measured on the height of the cube of the structure, so if the structure is 50 mm tall, you want to squash it to 25 mm tall.
Build a model with a displacement of -25 mm in the Y axis, with the plasticity material defined, and plot maximum Total Strain vs. displacement and also plot Reaction Force for your energy calculation. The ANSYS model will only be valid up to the point when the maximum Total Strain reaches 6%. After that point, some area of the model would have fractured in a physical test of a real sample, but the ANSYS model does not fracture. The material just keeps on stretching. Therefore, the Reaction Force for the displacement past the point when the Total Strain reached 6% will not represent reality and will be larger than a physical sample from that displacement onward.
Good luck on the next stage of your model building.
I am agree with you about this problem.But I think that the total strain of structure is not equal to strain of material(ribs).I think that if the strain of structure reaches to 50%,the strain of material reaches to 15-20%(roughly).And as you say ANSYS simulation do not estimate fracture of ribs,but I think differences of experimental data and simulation data will not be very large.
I should think about this problem,but at this time, we have 2 ways :
1.changing material and using from a polymer with larger plastic area and larger rupture strain.
2.simulation the fracture in ANSYS that I have no information and experiment about this.
You understand perfectly my point that 50% strain on the structure, which is equal to a 25 mm displacement of the top, might create a material strain in the ribs of some smaller value, but once the material strain has exceeded the rupture strain, the model is no longer predicting reality.
1. If you can find a material with a larger Elongation at Break (rupture strain), and ideally use the stress-strain curve for that material, then you can use the plasticity material model and if total strain is < elongation, then the computed Reaction Force will be valid for the 50% strain on the structure.
2. If you stay with a material with a low elongation and want to simulate the post fracture behavior, that can be done in ANSYS but it is complicated in Static Structural. One approach is to move the model into Explicit Dynamics which has element failure built into the solver by default. The down side is the extremely long solution times.
- All Categories
- Community Rules, Guidelines, and Tips
- News & Announcements
- Student Products
- Pre and Post Processing
- Physics Simulation
- Tutorials, Articles and Textbooks
- Installation and Licensing
- Student Competition Teams
- Site Feedback