General Mechanical

General Mechanical

contact pair command object

    • SaisudheerM
      Subscriber

      Hello all


      Can anyone provide an example of command object for contact pair


      Thank you

    • peteroznewman
      Subscriber

      Hello,


      What are you trying to achieve?  Are you using Mechanical Workbench?


      Do you already know how to create a contact pair?


      Regards,
      Peter

    • SaisudheerM
      Subscriber

      hi,


      I have created a contact pair in work bench, but i want to write a command object , i know bascis of APDL commands.can you please help me out how to write a command object script for generating contact pair in workbench, since i am loosing contact pair if i edit the geometry . so i want to give the command object .


      Thank you


       


       


    • peteroznewman
      Subscriber

      You don't need an APDL command.


      A Contact Region is automatically created between any set of faces that touch between adjacent bodies.


      Look in the Details Window when you click on the Contact Region item. You will see something like this:



      There may only be 1 face from each body. This example shows six faces on each body.


      The default contact is always Bonded.  You can change it to many other types, such as Frictional.


      There are several controls under the Advanced tab which can be used if the solver doesn't converge.

    • SaisudheerM
      Subscriber

      Hello Mr.Peter


      Apart from that without using those tools , Can i execute command object for creating contact pair .

    • peteroznewman
      Subscriber

      Hello, Saisudheer,


      I have never used a command object under a Contact so I have no idea what you would put there. Maybe some ANSYS person can reply.

    • SaisudheerM
      Subscriber

      Thank you, Mr Peter

    • jpasquerell
      Ansys Employee

      You can create a command object to add contact/target elements but it is recommended that you work in Mechanical APDL to figure out the commands as trying to create a command object especially one to create contact will likely take several iterations. 


      create a simple model then create a nodal component for for face or edge that will be the contact 


      create a nodal component for for face or edge that will be the target.


      Use *GET to get the maximum defined element type, material, and real constant set id


      select the contact component 


      create the element type for the contact using ET and KEYOPT with the id number being 1 greater than the existing max type id


      set the real and mat to be 1 above their max id values


      define the real constants for the contacts using the R, RMORE, RMODIF commands and the id of maxid +1


      issue ESURF to make the contacts


      select the target component


      create the element type for the targets using ET and KEYOPT with the id number being 2 greater than the existing max type id


      keep the same real and mat ids of 1 above their max id values


      issue ESURF to make the targets


       issue allsel to select everything


       


      Once the commands are good insert a command object under the Mechanical environment (such as Static Structural with this sequence so that the  contacts are made just prior to solving:


      fini


      /prep7


      ! commands to make contacts and targets


      finish


      /solu


       

    • SaisudheerM
      Subscriber

      Hello Mr JPASQUERELL


      Thank you so much I was looking for this type of solution.


      I will try it and let you know the.

Viewing 8 reply threads
  • You must be logged in to reply to this topic.