Hello all. I’m modeling random fiber inside concrete ( still in trials period). Let’s say I have 30 fiber and I need to use Link180 for all. Now I add command window for each to add the element type. Since I’m trying several options, it is really hard to keep doing that. Anyway I can do this in groups or in “bulk” for all fiber geometry? Thank you
Add same element type to several geometry
- 160 Views
- Last Post 06 August 2018
Here is a long discussion on how to create a large number of random fibers into DesignModeler for reinforcement of concrete.
The conclusion is that you can take a spreadsheet and read in bulk the coordinates of the endpoints of 30 fibers and they will become line bodies.
thank you for forwarding me to this discussion, it is helpful to see what is already available. I wrote my own matlab code and I have all points for lines. I'm asking about assigning "Link180" to each. Will that happened automatically, because I assign it now by inserting "command" for each one.
If you put a command object under each line body in Workbench, then you can assign the LINK180 element to that body. You can verify that it is working by using Tools > Write Input File in Mechanical and examining the contents of the file created.
Hopefully this analysis snippet is what you are after:
/prep7 !!! Setup for LINK180 area = 3.1414 et, 1010, 180 sectype, 1010, link secdata, area !!! Selects all beam188 elements for conversion to link180 esel, s, ename,, 188 emodif, all, type, 1010 emodif, all, secnum, 1010 !!! Revert back to solution /solu alls
write input file is gray and I can open it. but looking at the forum you referred made me thinking: what is the way you used to connect fiber with concrete as you mention there previously?
Appreciate your help
thank you for the code, that is exactly what I'm looking for. But where should I add this command in the tree?
Thank you Jason, That is way easier than copying the command fifty times
Slide 5 in Jason's link shows that you have to click on Solution, then the Write Input File will not be grey.
One way I know how to use line bodies that lie randomly within a solid volume as reinforcements is in the Explicit Dynamics solver where the Body Interactions tab allows the line bodies to be called out as type = Reinforcement.
This is rather elegant. The line bodies are meshed independently of the mesh of the solid volume. It is the solver that figures out which nodes of the line body is inside an element of the solid body, and connects those nodes to the intersecting solid elements. Below is a bit of the ANSYS help section.
184.108.40.206.4. Reinforcement Type
This body interaction type is used to apply discrete reinforcement to solid bodies. All line bodies scoped to the object will be flagged as potential discrete reinforcing bodies in the solver. On initialization of the solver, all elements of the line bodies scoped to the object which are contained within any solid body in the model will be converted to discrete reinforcement. Elements which lie outside all volume bodies will remain as standard line body elements.
The implicit solver used in Static Structural has a different way of dealing with reinforcement. I recall making sure the line body mesh shared nodes with the solid body mesh. Maybe some one else will comment on other methods available.
Could you please share the matlab code which you have used to model the fibers reinforcement? I am also working on the design and modeling of fibers in concrete in ANSYS workbench. I would like to follow your updates/progress in this matter.
- 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
- eMasters Degree from UPM
- Site Feedback