Ansys Employee

Hi Xiao,

Hopefully, this response is not too late. 

If you insert a command snippet to a part in Mechanical, in the comments of that snippet, you can see that MATID is the "material number used for this body".



The first row of command means defines an element type (ET). That element type ID is equal to MATID. What it does is to change your beam element type to "LINK180".  The second row is to change the key option of the link element. It is used to change some element related properties. However, LINK180 does not have keyopt(3), it only has keyopt(2) and keyopt(12) according to Ansys documentation I linked below. The third row defines a section type, which defines a LINK section type, and the type id is MATID. However, to make the model run, you still need another line to define the section area, like this:


area = 1

ET, matid, link180


sectype, matid, LINK



After you run the simulation, you can check the "Solution information"---> "Solver output" whether you have correctly defined the element type. You can also right-click on "Solution", ---> "Open solver file directory", there is a ds.dat file which is the input file. There, you can search matid and find its value. 


For more information about LINK180 element type, please refer to this documentation:https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v194/ans_elem/Hlp_E_LINK180.html?q=link180

A detailed description about element type can be found here: https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v201/en/ans_cmd/Hlp_C_ET.html

If you have trouble accessing the Ansys help, please refer to this post: https://studentcommunity.ansys.com/thread/how-to-access-the-ansys-online-help/