topic Re: Is there a way to automatically dimension derived from a solid thru Manage/Make Components part? in Inventor Forum

Is there a way to automatically dimension derived from a solid thru Manage/Make Components part?

inventor_man — Thu, 12 May 2022 15:42:49 GMT

The way we create sometimes our parts is to create solids within an .itp part for preliminary drawings and then convert each solid into separate .ipt by using Manage/Make Components option.

We use a template that uses L, W and T parameters and when creating a part we use the template so in the end the part derived from solid is based on the template with L, W, T set up for BOM. The problem is the derived part comes with 0's and in order to get proper dimensions to the part we need to draw sketches on it, dimension it and then use numbers on the sketched for L, W and T. Is there a way to automatically dimension derived from a solid thru Manage/Make Components part?

Re: Is there a way to automatically dimension derived from a solid thru Manage/Make Components part?

andrewiv — Thu, 12 May 2022 17:49:57 GMT

You could export the parameters from the original part to the derived part so the values are accessible in the new part. You won't be able to change them in the new part, but you can use them for equations, iProperties, etc..

Re: Is there a way to automatically dimension derived from a solid thru Manage/Make Components part?

MateriaGris — Thu, 12 May 2022 18:38:25 GMT

Hi @inventor_man

This rule combined with event triggers can be useful to you.

Dim Parte As PartDocument
Dim ParteComp As PartComponentDefinition
Dim Parametro As Inventor.Parameter
Dim ParametroDeriv As DerivedParameter
Dim ParametrosDerivados As DerivedParameters

Try
		Parte = ThisDoc.Document
		ParteComp = Parte.ComponentDefinition
		PrametrosDerivados = ParteComp.Parameters.DerivedParameterTables.Item(1).DerivedParameters
		ParametroDeriv = PrametrosDerivados.Item(1)
		
		For Each ParametroDeriv In PrametrosDerivados
			
			For Each Parametro In ParteComp.Parameters.UserParameters
				
				If Left(ParametroDeriv.Name,1) = Parametro.Name Then
					Parametro.Expression =ParametroDeriv.Name
				End If
				
			Next
			
		Next
Catch
	
End Try

I enclose files applying what is detailed here, in my case the parameter names I used are L, U, P, it does not allow me to use L, W, T due to conflict with the unit system.

In your template, in addition to this rule, you must have the previously generated user parameters (L,W,T) all with a value of 0.

You will also need to configure the event trigger so that this rule is executed automatically, in this case I suggest you configure "Part geometry change".

When you derive your reference file, make sure to export the parameters you mention (L,W,T)

This rule will be based on the first letter of the name of each parameter, to compare derived parameters with user parameters.

Inventor by default, if the parameter name already exists, adds _1 or the corresponding number, that is, the user parameters would be L, W, T and the derived parameters would be L_1, W_1, T_1.

I hope you find it useful, if so, please mark it as answer.

Have a great day!

Re: Is there a way to automatically dimension derived from a solid thru Manage/Make Components part?

SBix26 — Thu, 12 May 2022 19:08:13 GMT

Following up on @andrewiv 's post, here is how you export parameters from the master file:

Parameters checked for export in the master file are then available in the Derive Part dialog to be selected for deriving into the part file.

Sam B

Inventor Pro 2023.0.1 | Windows 10 Home 21H2