Creating Formulas to form Parametric model | CATIA V5
December 1, 2023 2024-11-11 14:22Creating Formulas to form Parametric model | CATIA V5
Overview
In this Tech Tip, you will learn about Parametric model. How to rename the Parameters in an Existing CATIA V5 Model and Create Formulas for the same Parameters.
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Please follow the below steps to achieve the required result –
Step 1:
Open the CATIA Part named Bolt.CATPART.
Step 2:
Make sure that you are on Part design Workbench.
Select Tools | Options | Infrastructure | Part Infrastructure | Display. Activate Parameters, Relations to Display in Specification Tree.
Step 3:
Select Tools | Formula or Select Knowledge Toolbar > select Formula.
Step 4:
Select New Parameter of Type to add new parameter, select Length as type, Enter name as Bolt_Dia, Value as 50mm
Click Ok.
Step 5:
To add Relations, Select Sketch1 in the specification Tree. Right click on the Dimension as Shown select Rename Parmeter.
Enter Parameter name as Hex_length, Right click on the value select Edit Formula.
Edit formula as Bolt_Dia*1.2 and Click Ok to create Relation.
Notice that Formula.1 has been created and displayed in the specification tree.
Step 6:
Click on Update icon to update the parameter value.
Step 7:
Similarly change the name for remaining parameters and adding formulas.
For Pad.1 rename as Pad, Formula as 0.7*Bolt_Dia
Step 8:
Click on Sketch.4 under Shaft.1, Right click on the Dimension Rename Parameter as shown below.
Rename as Bolt_Radii, Edit the formula, Enter Bolt_Radii= Bolt_Dia/2. Click Ok to display in Specification Tree.
Similarly,
Rename length as Shank_Length, Edit the formula, Enter Shank_length=(Bolt_Dia+10mm)*3. Click Ok to display in Specification Tree.
Step 9:
Click on Update icon to update the parameter value.
Step 10:
Change the Value of the Parameter Bolt_Dia according to that parametric model will be Updated.
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