iLogic code to create a User Parameter

Anonymous · ‎07-29-2011

I want to use iLogic to create User Parameters with Multi-Value lists filled with info from an excel spreadsheet. What is the code to create a new User Parameter? I can't seem to find it in the help wiki.

Thanks!

ravikmb5 · ‎07-30-2011

@Anonymous wrote:
I want to use iLogic to create User Parameters with Multi-Value lists filled with info from an excel spreadsheet. What is the code to create a new User Parameter? I can't seem to find it in the help wiki.

Thanks!

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oMyParameter=ThisApplication.ActiveDocument.ComponentDefinition.Parameters.UserParameters
'Setting an userParameter as inches
oParameter=oMyParameter.AddByExpression("Length_inch", "3", UnitsTypeEnum.kInchLengthUnits)
oParameter=oMyParameter.AddByExpression("Width_inch", "3", "in")

'Setting an userParameter as Millimeteres
oParameter=oMyParameter.AddByExpression("Length_mm", "3", UnitsTypeEnum.kMillimeterLengthUnits)
oParameter=oMyParameter.AddByExpression("Width_mm", "3", "mm")

'Setting an userParameter as text parameter
oParameter=oMyParameter.AddByValue("color", "bule", UnitsTypeEnum.kTextUnits)
oParameter=oMyParameter.AddByValue("color", "red", UnitsTypeEnum.kTextUnits)
oParameter=oMyParameter.AddByValue("color", "yellow", UnitsTypeEnum.kTextUnits)

the above example creates single user parameters

but i dont know wheteher there is a way to create a Multi-value user parameter

Please mark this response as Problem Solved if it answers your question.
----------------------------------------------------------------------------------------------
Ravi Kumar MB,
HP Z220 SFF Workstation
Autodesk Inventor Certified professional 2016
Email: [email protected]

Anonymous · ‎08-01-2011

Thank you Ravi. That works.

Anonymous · ‎08-14-2013

it's possible to try,catch and add a user parameter in each parts of assembly with ilogic???

ekinsb · ‎08-20-2013

Take a look at this blog post for some help with updating parts associated with an assembly.

http://modthemachine.typepad.com/my_weblog/2013/08/updating-parts-through-an-assembly.html

Brian Ekins
Inventor and Fusion 360 API Expert
Mod the Machine blog

Anonymous · ‎09-16-2014

oMyParameter=ThisApplication.ActiveDocument.ComponentDefinition.Parameters.UserParameters
oParameter=oMyParameter.AddByValue("Material", "Steel, S275", UnitsTypeEnum.kTextUnits)
MultiValue.SetList("Material", "Keruing Board", "Aluminum 1050", "Aluminum Alloy 5251", "Aluminum Alloy 5454 h22", "Aluminum 6061", "Domex 460 MCD", "DX51D Z275", "GRP", "Nylon 6/6", "Plywood, Finish", "Rubber", "Rubber EPDM", "Steel, S275", "Steel, S275JR", "Steel, S355", "Steel, S355J0", "Steel, S355J2+N", "Steel, S355JR")

for example creates multi value parameters

Anonymous · ‎10-21-2014

Thanks ravikmb5 your rule works wel when I run it as an external rule. But how can I make it work without having to open the part. I.e in edit mode so the parameter is created in the part being edited. At the moment it creates the parameter but in the assembly.

Here is how i changed it:

SyntaxEditor Code Snippet

oMyParameter=ThisApplication.ActiveDocument.ComponentDefinition.Parameters.UserParameters
'Setting an userParameter as text parameter
oParameter=oMyParameter.AddByValue("JOB_NUMBER", "", UnitsTypeEnum.kTextUnits)
oParameter=oMyParameter.AddByValue("JOB_DESCRIPTION", "", UnitsTypeEnum.kTextUnits)

Regards
Andrew

ravikmb5 · ‎04-23-2015

@Anonymous wrote:

Thanks ravikmb5 your rule works wel when I run it as an external rule. But how can I make it work without having to open the part. I.e in edit mode so the parameter is created in the part being edited. At the moment it creates the parameter but in the assembly.

edit mode

i guess u are in assembly mode......

do u want to create part parameters from assy

Please mark this response as Problem Solved if it answers your question.
----------------------------------------------------------------------------------------------
Ravi Kumar MB,
HP Z220 SFF Workstation
Autodesk Inventor Certified professional 2016
Email: [email protected]

Anonymous · ‎04-23-2015

Thanks for your reply.....

Yes, I am in the .iam and want to run a rule to insert custom parameters into the parts to automatically change the "Project" parameter by entering a value in a form, but at the moment I have to open every part to copy and run the rule. In stead of just double clicking on the part and running the rule.

Logos_Atum · ‎04-07-2016

@ravikmb5

Hello Ravik,

that just saved my day. I tried to get to know the internal name for the parameter - tried to "call",

well tried and tried to declare a parameter existing as a value to copy the value... also tried to declare,

yet got to a lambada error message. Declaring the open document was part of the idea.... yet.

I am not skilled at all.

Can I ask for the reference you´re using?

And thank you very much for making that work.

Dogs aren´t flammable.

ravikmb5 · ‎04-09-2016

oUserParams.AddByExpression("EXPRESSION", _
Inventor.UnitsTypeEnum.kUnitlessUnits)

U CAN USE THIS FOR ADDING BY EXPRESSION

Please mark this response as Problem Solved if it answers your question.
----------------------------------------------------------------------------------------------
Ravi Kumar MB,
HP Z220 SFF Workstation
Autodesk Inventor Certified professional 2016
Email: [email protected]

Logos_Atum · ‎04-09-2016

MORBO SEND HIS REGARDS TO YHE HUMAN WYRMIN

:))))))

Dogs aren´t flammable.

cencinaNB2ET · ‎07-18-2017

Yes,

what needs to change to work in an Assembly?

Thanks

cencinaNB2ET · ‎07-18-2017

I got it... sorry I added a version of Brian Ekins Code

Dim Doc As AssemblyDocument

Doc = ThisApplication.ActiveDocument

Dim userParams As UserParameters

Dim param As Parameter

userParams = Doc.ComponentDefinition.Parameters.UserParameters

param = userParams.AddByValue("Name_User_Parameter","SomeValue",UnitsTypeEnum.kTextUnits)

For Each oPara As Parameter In userParams

Dim oName As String = oPara.Name

If oName = " Name_User_Parameter _1" Then

oPara.Delete

End If

Next

DeerSpotter · ‎08-15-2018

i dont think a lot of people understand how much this is a gold mine.

Here is my end result of how i used your code:

Dim Doc As AssemblyDocument
Doc = ThisApplication.ActiveDocument
Dim userParams As UserParameters
Dim param As Parameter 
 
userParams = Doc.ComponentDefinition.Parameters.UserParameters
param = userParams.AddByValue("PUMP_MATERIAL", "CAST IRON", UnitsTypeEnum.kTextUnits)
 
For Each oPara As Parameter In userParams
Dim oName As String = oPara.Name
If oName = "PUMP_MATERIAL_1" Then 
oPara.Delete
End If
Next

'set list of values
MultiValue.SetList("PUMP_MATERIAL", "CAST IRON", "STAINLESS")

'Dim booleanParam As Object
standard = InputRadioBox("Select a Material", _
"CAST IRON", "STAINLESS", True, Title := "iLogic") 

If standard = True Then
Parameter("PUMP_MATERIAL") = "CAST IRON"
Else
Parameter("PUMP_MATERIAL") = "STAINLESS"	
End If

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cencinaNB2ET · ‎08-16-2018

Yes That's Right

You can have more control over your files this way.

Here is the code you posted, I added a few things.

SyntaxEditor Code Snippet

Dim oAsmDoc As AssemblyDocument 
oAsmDoc = ThisDoc.Document
Dim oAsmDef As AssemblyComponentDefinition
oAsmDef = oAsmDoc.ComponentDefinition
Dim param As Parameter
Dim userParams As UserParameters
userParams = oAsmDef.Parameters.UserParameters
Dim All_New_Parameters As New ArrayList





For Each oPara As Parameter In userParams
If oPara.Name = "PUMP_MATERIAL" Then 
GoTo Skip_Creation
End If
Next


Dim Options_Available As New ArrayList
Options_Available.Add("CAST IRON")
Options_Available.Add("STAINLESS")



oParameter = userParams.AddByValue("PUMP_MATERIAL", Options_Available(0), UnitsTypeEnum.kTextUnits)
MultiValue.List("PUMP_MATERIAL") = Options_Available
MultiValue.SetValueOptions(True, DefaultIndex := 0, NumericCompare := "=")
All_New_Parameters.Add("PUMP_MATERIAL")





Skip_Creation :
 
 

Dim standard As Boolean
standard = InputRadioBox("Select a Material", "CAST IRON", "STAINLESS", standard, Title := "iLogic")


If standard = True Then
Parameter("PUMP_MATERIAL") = "CAST IRON"
Else
Parameter("PUMP_MATERIAL") = "STAINLESS"	
End If







''''' Just in Case you have more copies - Delete them

Dim Copies_To_Delete As New ArrayList
For t = 0 To All_New_Parameters.Count - 1
Copies_To_Delete.Add(All_New_Parameters(t) + "_1")
Copies_To_Delete.Add(All_New_Parameters(t) + "_1" + "_2")
Next t

For Each oPara As Parameter In userParams
If Copies_To_Delete.Contains(oPara.Name) Then
oPara.Delete
End If
Next





iLogicVb.UpdateWhenDone = True

DeerSpotter · ‎08-17-2018

Thank you for sharing your knowledge.

This is going to change every thing for me for all my ilogic coding.

Dim oDoc As AssemblyDocument = TryCast(ThisDoc.Document, AssemblyDocument)
Dim compDef As AssemblyComponentDefinition = oDoc.ComponentDefinition

If Parameter("PUMP_MATERIAL") = "CAST IRON" Then
For Each oComp In compDef.Occurrences
	For Each oConstraint In oComp.Constraints
		If kPartDocumentObject Then
			If iProperties.Value(oComp.Name, "Project", "Description") = "CASTIRONSTATOR" Then
				oComp.Visible = True 'turn on
			End If
			If iProperties.Value(oComp.Name, "Project", "Description") = "STAINLESSSTATOR" Then
				oComp.Visible = False 'turn off
			End If
			If iProperties.Value(oComp.Name, "Project", "Description")="CASTIRON" Then
				If oConstraint.Name = "VERTICALCI" Then
					oComp.Visible = True
					iProperties.Value("Custom", "Orientation")="VERTICAL"
				End If
				If oConstraint.Name = "RIGHTCI" Then
					oComp.Visible = False
				End If
				If oConstraint.Name = "LEFTCI" Then
					oComp.Visible = False
				End If
			End If
			If iProperties.Value(oComp.Name, "Project", "Description")="STAINLESS" Then
				If oConstraint.Name = "VERTICALSS" Then
					oComp.Visible = False
				End If
				If oConstraint.Name = "RIGHTSS" Then
					oComp.Visible = False
				End If
				If oConstraint.Name = "LEFTSS" Then
					oComp.Visible = False
				End If
			End If
		End If
	Next	
Next
End If

If Parameter("PUMP_MATERIAL") = "STAINLESS" Then
For Each oComp In compDef.Occurrences
	For Each oConstraint In oComp.Constraints
		If kPartDocumentObject Then
			If iProperties.Value(oComp.Name, "Project", "Description") = "STAINLESSSTATOR" Then
				oComp.Visible = True 'turn on
			End If
			If iProperties.Value(oComp.Name, "Project", "Description") = "CASTIRONSTATOR" Then
				oComp.Visible = False 'turn off
			End If
			If iProperties.Value(oComp.Name, "Project", "Description")="STAINLESS" Then
				If oConstraint.Name = "VERTICALSS" Then
					oComp.Visible = True
					iProperties.Value("Custom", "Orientation")="VERTICAL"
				End If
				If oConstraint.Name = "RIGHTSS" Then
					oComp.Visible = False
				End If
				If oConstraint.Name = "LEFTSS" Then
					oComp.Visible = False
				End If
			End If
			If iProperties.Value(oComp.Name, "Project", "Description")="CASTIRON" Then
				If oConstraint.Name = "VERTICALCI" Then
					oComp.Visible = False
				End If
				If oConstraint.Name = "RIGHTCI" Then
					oComp.Visible = False
				End If
				If oConstraint.Name = "LEFTCI" Then
					oComp.Visible = False
				End If
			End If
		End If
	Next	
Next
End If

i have it then set for all the buttons the same way (left, right, vertical). This way i control all of my model types through a simple form.
Hope that i possibly showed you something as well. 🙂

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Biju.Veedu · ‎07-21-2021

Hi,

is there any ilogic rule available to creating user parameters in flat pattern stage ?

WCrihfield · ‎07-22-2021

Hi @Biju.Veedu .

While in that Flat Pattern mode/environment, you can still create user parameters manually, and so you can still create them by code the same way too, but when done by code, they just don't shop up right away in the parameters dialog box. Once you go back to the normal folded part mode/environment then you can see that the user parameter you created by code while in Flat Pattern mode was really created.

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Biju.Veedu · ‎07-22-2021

@WCrihfield thanks for the info. but I want to stay that parameters at flat stage. Manually typing each one is very painful.

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iLogic code to create a User Parameter

iLogic code to create a User Parameter

iLogic code to create a User Parameter