Changing element type in Ansys Workbench

[nabeel1968]

Dear friends
I am using Ansys Workbench (AWB) to simulate my hybrid beam model (composed of concrete deck and GFRP section (I-shaped). Then I save the file as ---.dat (from: Tools --- Write Input File) to read it from APDL and analyze it.
As I know, AWB selects element types that best suit the model components engineering data (material properties). But when one wants to change the element type, a “Command” should be inserted for the desired part of model. What I did in my job is the following:
.One engineering data (default material, i.e, structural steel) is kept.
.When I opened (AWB Mechanical), I inserted a “Command” to select the SOLID65 for concrete deck and SHELL181 for glass fiber-reinforced polymer (GFRP) section, as follow:
For SOLID65 (concrete)
ET,MATID,SOLID65
R,MATID,0,0,0,0,0,0
RMORE,0,0,0,0,0
MP,EX,MATID,28000
MP,PRXY,MATID,0.2
For SHELL181 (GFRP)
ET,MATID,SHELL181
R,MATID,0,0,0,0,0,0
RMORE,0,0,0,0,0
MP,EX,MATID,17900
MP,PRXY,MATID,0.33
.When I fulfilled the entire items and click solve, I got the following error message:
Element type 1 is the not the same shape as SOLID65. Element type can’t be changed while element type 1 exist. I got the same for SHELL181.
Please advise urgently.
Regards.

 

[STpipe]

I'm having trouble understanding what you have been doing to isolate the source of your error. At first you mentioned that you generated an input file from Workbench which you then intend to use in Ansys Classic, correct? If that's the case, shouldn't you be able to see the material and property assignments directly in that input file (using a simple text editor) and modify them as needed to run your analysis in APDL?

In the second part, you mention inserting commands in Workbench Mechanical. Where did you insert the custom command exactly? Is it within the geometry environment or the solution(?) environment?

In my experience, this is what I would have done to override the element type in Workbench Mechanical(or any of the other properties).

1) In the geometry environment, insert a command in the bodies for the concrete:

rc_conc = matid !Assigns material id number for concrete body to variable rc_conc

2) Similar to the above, do the same for the bodies (surfaces) that represent the GFRP:

gfrp = matid !Assigns material id number for GFRP to variable gfrp

3) In the solutions(? - sorry don't have Workbench access right now so I'm basing this off memory) part of the tree, insert a command that will overwrite the default properties:

!For SOLID65 (Concrete)
ET,rc_conc,SOLID65
R,rc_conc,0,0,0,0,0,0
RMORE,0,0,0,0,0
MP,EX,rc_conc,28000
MP,PRXY,rc_conc,0.2

!For SHELL181 (GFRP)
ET,gfrp,SHELL181
R,gfrp,0,0,0,0,0,0
RMORE,0,0,0,0,0
MP,EX,gfrp,17900
MP,PRXY,gfrp,0.33

Depending on where and how you inserted your custom command, Ansys could be using a value matid from another element type that's incompatible with your concrete solid and gfrp shell, hence the error.

What I believe happens is that every body (body, surface, lines) gets assigned a number matid which just gets added on as the program cycles through all the bodies. Each body is assigned a material, element, real constant etc. number based on that matid value. So by doing steps #1 and #2, you assign that number (which you can't see by default) to a variable which you later call upon and use in Step #3 to overwrite the material properties.
See if you have any luck with this, or provide additional information on the nature of your problem.

 

[Mr.Milhouse]

Hello guys,

I just started using ANSYS, so excuse my amateur questions. After creating the geometry of a Wall I tried to change Element Typ with a Command. I typed follow:
ET,matid,SHELL183
KEYOPT,matid,3,3
The solution of the Mises Stress looks the same as if I did not change Element Typ afterwards. Does this mean my default Element Typ was the same as my manuel typed one? The only Information a get about the Element with default Settings is the Element Typ is a Quad8. Can somebody please tell me how I figure out if this is the same as SHELL183? I also tried to change the ElemtTyp to:
ET,matid,SHELL182
KEYOPT,matid,3,3
If I do that the stress solution shows me a stress of 0 in the entire body. How come? And if I change SHELL182 to SOLID185 an unknown error appearse. Someone any Idea, why?
I were very glad if someone might answer my three questions.
Regards