Autodesk Inventor

[#1]

I would like to have a rule that will add specific user parameters to a part file.  These parameters need to be formatted so the width, depth and thickness will control the description of the part.

IE:

Width=4

Depth=2

Thickness=3/16

DESCRIPTION = TS <Width>X<Depth>X<Thickness>

I would like to format each parameter so that the:

Format=Fractional

Precision=1/16

Unit string=False

This is what I have so far:

 oMyParameter=ThisApplication.ActiveDocument.ComponentDefinition.Parameters.UserParameters
 
 oParameter=oMyParameter.AddByExpression("Width", "TOP_RAIL_WIDTH", UnitsTypeEnum.kInchLengthUnits)
  oParameter.ExposedAsProperty=True
 oParameter.Units="in" 
 
 oParameter=oMyParameter.AddByExpression("Depth", "TOP_RAIL_DEPTH", UnitsTypeEnum.kInchLengthUnits)
 oParameter.ExposedAsProperty=True
 oParameter.Units="in"
 
 oParameter=oMyParameter.AddByExpression("Thickness", "TOP_RAIL_THICKNESS", UnitsTypeEnum.kInchLengthUnits)
 oParameter.ExposedAsProperty=True
 oParameter.Units="in"

The TOP_RAIL parameters are from a linked file.

Thanks,

Brian

[#2]

just put a check in the export box in the parameters. for the format after you put a check mark in the export box if you go over to the equation right click you wil have new options. One is custom property format in there you can change the output.....

[#3]

Oh and you don't really need ilogic..

[#4 · Accepted solution]

Hi brian

Here is some iLogic code and an example file that will format parameters and add them to the Description iProperty.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

Dim oWidth, oDepth, oThickness  As Parameter
Dim oFormat As CustomPropertyFormat

oWidth = Parameter.Param("Width")
oWidth.ExposedAsProperty = True
oFormat=oWidth.CustomPropertyFormat
oFormat.PropertyType=Inventor.CustomPropertyTypeEnum.kTextPropertyType
oFormat.Precision=Inventor.CustomPropertyPrecisionEnum.kSixteenthsFractionalLengthPrecision
oFormat.Units="in"
oFormat.ShowUnitsString=False

oDepth = Parameter.Param("Depth")
oDepth.ExposedAsProperty = True
oFormat=oDepth.CustomPropertyFormat
oFormat.PropertyType=Inventor.CustomPropertyTypeEnum.kTextPropertyType
oFormat.Precision=Inventor.CustomPropertyPrecisionEnum.kSixteenthsFractionalLengthPrecision
oFormat.Units="in"
oFormat.ShowUnitsString=False

oThickness = Parameter.Param("Thickness")
oThickness.ExposedAsProperty = True
oFormat=oThickness.CustomPropertyFormat
oFormat.PropertyType=Inventor.CustomPropertyTypeEnum.kTextPropertyType
oFormat.Precision=Inventor.CustomPropertyPrecisionEnum.kSixteenthsFractionalLengthPrecision
oFormat.Units="in"
oFormat.ShowUnitsString=False

iProperties.Value("Project", "Description") = "= TS <Width> x <Depth> x <Thickness>"

[#5]

Curtis,

It works great.

Thanks,

Brian

[#6]

Hi brian, 

I'm glad to hear that worked.

I noticed that I left those first two lines of the code in. They're not really needed, and don't really do anything as written because  those things get defined later in the code. They were just vestiges of my first attempt that I forgot to remove once I went a different way.  I just thought I'd mention it in case it confuses someone who happens upon this in the future.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

so, this works just as well:

oWidth = Parameter.Param("Width")
oWidth.ExposedAsProperty = True
oFormat=oWidth.CustomPropertyFormat
oFormat.PropertyType=Inventor.CustomPropertyTypeEnum.kTextPropertyType
oFormat.Precision=Inventor.CustomPropertyPrecisionEnum.kSixteenthsFractionalLengthPrecision
oFormat.Units="in"
oFormat.ShowUnitsString=False

oDepth = Parameter.Param("Depth")
oDepth.ExposedAsProperty = True
oFormat=oDepth.CustomPropertyFormat
oFormat.PropertyType=Inventor.CustomPropertyTypeEnum.kTextPropertyType
oFormat.Precision=Inventor.CustomPropertyPrecisionEnum.kSixteenthsFractionalLengthPrecision
oFormat.Units="in"
oFormat.ShowUnitsString=False

oThickness = Parameter.Param("Thickness")
oThickness.ExposedAsProperty = True
oFormat=oThickness.CustomPropertyFormat
oFormat.PropertyType=Inventor.CustomPropertyTypeEnum.kTextPropertyType
oFormat.Precision=Inventor.CustomPropertyPrecisionEnum.kSixteenthsFractionalLengthPrecision
oFormat.Units="in"
oFormat.ShowUnitsString=False

iProperties.Value("Project", "Description") = "= TS <Width> x <Depth> x <Thickness>"

[#7]

sir can anyone help me to update the thickness of a sheet metal,  through custom properties in BOM(Assembly level)

if i create opposite hand of a part the thickness will not getting updated please help me out update through custom properties, i want like if i update the custom properties thickness then automatically it has to get updated in parameters.

thanks and regards

Manjunatha

[#8]

sir, can you help me create co to remove All Custom property?

i want to clearup all custom properties and add new one.

Thanks and regard

[#9]

Remove directly from iproperties.

[#10]

Create the opposite hand using derived component. Derive a mirror part and bring the parameters of the original. This way both thicknesses will get updated.