topic Re: Reference constrains in assembly in Inventor Forum

Reference constrains in assembly

Anonymous — Thu, 15 Nov 2018 13:14:14 GMT

I would like to have reference measure (constrains) in an assembly, so then I change a driven constrains I can read the "output" in the reference measure.

A simple example: A linkage of four parts has an angle constrain A that I would like to use as a driven measure. If I put in constrain B my system it would be over-constrain BUT I would like to put it in so I can get the output measure.

I will then use a script to change A and plot the output "signal" B to an excelsheet. The CAD will work like a calculator to solve an advanced geometry problem.

If I work with a sketch this would be possible but the problem/case I work with now is in 3d so I need assembly mode.

Hope you understand.

Goran

Re: Reference constrains in assembly

Cadmanto — Thu, 15 Nov 2018 13:41:39 GMT

Goran,

If you dimension your sketch correctly, you can add the dimensions to fully constrain it without the angle dimension. Then you can still add the angle dimension. It will prompt you basically stating you don't need it and do you want to add it as a reference dimension anyway, to which you would say "Yes".

It will be added showing it as reference.

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Re: Reference constrains in assembly

JDMather — Thu, 15 Nov 2018 13:55:09 GMT

....there is also a toggle for Reference dimensions in the upper right area of you sketch ribbon.

Once this (reference) dimension is in place - you will get exactly the behavior that you describe.

Re: Reference constrains in assembly

JBEDsol — Thu, 15 Nov 2018 14:25:00 GMT

I assume the issue is that you have a bunch of parts in an assy and want things read from their assembly positions, not a sketch that you have resembling the screenshot provided.

You could add an assy sketch but I usually have at least a little trouble w/ assy sketches whenever things update.

Maybe add a "ghost" part where you use "Add Component" and put the face of what you want to measure into that component. You could use that part w/ iLogic or add a sketch and put in a reference dimension. Unfortunately the data would be in the part you've added and not the assy it'self but you could use some iLogic to read a custom parameter into your assy from that part.

Re: Reference constrains in assembly

Anonymous — Fri, 16 Nov 2018 07:27:11 GMT

Hi JBEDsol

Thanks for your answer. You understood what I was looking for in the assembly mode NOT the part-sketch as I wrote.

But I am not sure what your solution is. I have tried a sketch with projected lines in assembly mode but those lines will be anchored so they will not be updated. You wrote something about a ghostpart and "add component" and I am not sure how this will work. Please explain.

BR/Goran

Re: Reference constrains in assembly

Anonymous — Mon, 19 Nov 2018 07:16:40 GMT

Hi JBEDsol

Thanks for your answer. You understood what I was looking for in the assembly mode NOT the part-sketch as I wrote.

BR/Goran

Re: Reference constrains in assembly

kelly.young — Mon, 19 Nov 2018 22:21:39 GMT

Hello @Anonymous I understand that you want to control your setup from the Assembly level. You could setup an Adaptive Assembly Sketch but as stated the links can become problematic and break if not setup perfectly.

Alternatively, you could create a base part sketch that will dive all the other parts using Derive. Then create a quick iLogic Rule to change the size through a Form.

If all the parts are derived off the same base part sketch you don't have to use any Constraints in the Assembly, just Ground & Root all the parts.

See the attached setup and if that helps give you an idea of how to control it a bit easier.

Please select the Accept Solution button if a post solves your issue or answers your question.

Re: Reference constrains in assembly

Anonymous — Tue, 20 Nov 2018 14:47:25 GMT

Hi Kelly

I finally manage to solve my problem. I used a "base/ghost" part there I copy those surfaces I was interesed from the assy. I could then create sketches in that part and recall those parameters in the IL-script. So thank you for your tip.

But I had a show-stopper, I could not understand until I found out that my excel has 32-bit and Inventor 64-bit. Re-install excel and now it work. (Thanks for a tip in this forum)

I still have a question: How could i erase my excel sheet before I start to send data to it in my IL-code?

Below a paste-snip of the code.

/Goran

    iLogicVb.UpdateWhenDone = True
    ThisApplication.ActiveDocument.Update()

    t=1+i-start_vinkel
    column_Vinkel = "A" & t+1
    column_Send_X = "B" & t+1
    column_Send_Y = "C" & t+1
    column_Mottag_X = "D" & t+1
    column_Mottag_Y = "E" & t+1
    GoExcel.CellValue(ExcelFile, "Ark1",column_Vinkel) = i
    GoExcel.CellValue(ExcelFile, "Ark1",column_Send_X) = Parameter("Part13:1", "d0")

Re: Reference constrains in assembly

kelly.young — Tue, 20 Nov 2018 18:37:33 GMT

@Anonymous here are a few links that should point you in the right direction.

Ilogic code to export BOM to excel file overwrites data in excel file

Inventor Trenches: Create a New Excel File with iLogic

How to create a excel file using ilogic?

For further iLogic inquiries post at Inventor Customization Forum for best results.

Please select the Accept Solution button if a post solves your issue or answers your question.