How to make option mode parameter in Catia
Hi, does anyone know how to make this kind of parameter in Catia where I can set different value for different type of let say length of metal rods. Let say that Mode "0 mm" represent length of 200 mm and Mode "1 mm" represent length of 100 mm.
Ozgur I found solution tnx anyway hope it will help somebody later :)
Tools -> Options -> Part Infrastructure -> Display ->Check Parameters(Relations and constrains if needed)
Click on Formula on the knowledge toolbar.
Change Filter Type to User Parameters.
Under New Parameter of Type Shift from Single Value to Multiple Values.
A pop up will open asking you to enter values, enter as many values as you want.
Click on New Parameter of Type now.
A Parameter with default name will add to list.
Highlight that Parameter and Edit the name in the Textbox next to New Type of Parameter.
Now in the tree under Parameters you will see your new Parameter with Multiple values.
Make a profile and click on Pad Option
In the textbox where you enter Dimension values right click and you will find an option called Edit Formula ,click it.
In the Textbox after “=“ sign type the name of your Parameter ,Click Ok.
Now your Parameter is linked to Dimension value of the Pad.
Double click on the parameter on the tree and the toolbar like you have presented in the question will open with the values you have provided as a dropdown.
Vary the values and the Dimension varies accordingly after updation.
In the example that you have shown he has used a boolean type of Parameter to vary the occurrence of an activity. Eg: 1 Pad happens, 0 Pad doesn't happen.