Learning Forum

[SaisudheerM]

Hello all

Can anyone provide an example of command object for contact pair

Thank you

[peteroznewman]

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]

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]

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]

Hello Mr.Peter

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

[peteroznewman]

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]

Thank you, Mr Peter

[jpasquerell]

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]

Hello Mr JPASQUERELL

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

I will try it and let you know the.