October 26, 2018 at 8:14 amtanmaynadeSubscriber
I am facing issues with my program. Listed below. This is form my masters project. Also in what way can I connect the filleted surfaces shown in fig by a weld or just load or stress transfer connection. The link to the program is
October 27, 2018 at 9:08 pmVitaliy_DegtyarevSubscriber
You can find more detailed descriptions of the issues in the jobname.err file in the working directory. When I ran your code, I got a warning about only one element violating shape warning limits. The following description was given:
Quadrilateral element 41288 has a pair of opposite edges that are
77.42 degrees away from being parallel. This exceeds the warning
limit of 70 degrees.
You can still run the analysis with this warning, but it is better to change the mesh. I usually select lines and divide them as needed using the LESIZE command, after which I mesh my models using mapped meshing (the MSHKEY command). With this method you have more control over the mesh and get a nice mesh with only rectangular and square elements. You may also want to have smaller divisions for the radii.
If your connections are discrete, you can couple displacements of the nodes that need to be connected using the CP command. If the connections are continuous, you could specify bonded contact between the surfaces.
Hope this helps.
November 23, 2018 at 1:23 pmtanmaynadeSubscriber
how to do bonded contact
November 23, 2018 at 1:45 pmRohith PatchigollaAnsys Employee
I have created a simple example to create contacts between two blocks in apdl. It is well commented.
You can understand the basic procedure here and can further apply it to your model.
Also, please go through the help documentation for more reference on any commands used in the script.
block,0,1,0,1,0,1 !make two blocks touching each other
et,1,186 !define a solid element type
mp,ex,1,100 !define some elastic material properties
esize,0.2 !element size
vmesh,all !mesh all volumes
et,2,174 !create contact elements
keyopt,2,12,5 !bonded contact
r,2 !real number for this contact pair
et,3,170 !create target elements
asel,s,,,6 !select contact area
nsla,s,1 !select nodes attached to this area
esln !select elements attached to the selected nodes
type,2 !set contact type number
real,2 !set real number for contact pair - one real number for each contact pair
esurf !create contact elements on selected nodes
asel,s,,,11 !select target area
type,3 !set target element type number
real,2 !set real number for this contact pair
esurf !create target elements
nsel,s,loc,x,0 !constrain one end of block 1
nsel,s,loc,x,2 !apply displacement on other end of block 2
plnsol,u,x !plot disp x
You can also do this process via ANSYS Classic GUI using Contact wizard.
Hope this helps.
November 23, 2018 at 4:23 pmtanmaynadeSubscriber
thanks a lot
November 23, 2018 at 4:24 pmtanmaynadeSubscriber
also, I'm not able to create e proper mesh for my original program some elements get out of shape?
November 26, 2018 at 3:14 pmRohith PatchigollaAnsys Employee
Please provide some mesh sizing controls (to refine the mesh at these areas) to get a proper mesh. Also, posting an image of your mesh, where the elements get out of shape would help us provide better suggestions.
November 26, 2018 at 4:26 pmSandeep MedikondaAnsys Employee
Please create a new discussion for your question. This discussion is closed. Take a moment to review the guidelines on the Student Community.
- 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.