topic Re: Reference dimension in Inventor Programming Forum

Reference dimension

madstrolle — Fri, 12 May 2023 11:26:49 GMT

Hi,

We often draw square profiles and other parts dimensions that isn't editable. On these profiles we want these dimensions to be, reference dimensions e.g. (50).

Is there a way to do this automatically?

Regards

Re: Reference dimension

CCarreiras — Fri, 12 May 2023 11:36:24 GMT

Can you explain better what's your goal?

If you already create the dimensions, You can toggle any ordinary dimension into a reference dimension (and vice-versa)

Select them and click here:

If you are about to create the dimensions, You can turn on the button first and then create the dimensions, the dimensions will be all reference dimensions

Re: Reference dimension

madstrolle — Fri, 12 May 2023 11:40:47 GMT

It's when i'm making a 2D drawing. See picture

Re: Reference dimension

madstrolle — Fri, 12 May 2023 12:14:21 GMT

If I do that way, I can't change the size in my Ilogic form.

Re: Reference dimension

Frederick_Law — Fri, 12 May 2023 13:10:32 GMT

Maybe use Basic.

If not, set up a Style for Reference Dimension.

Re: Reference dimension

madstrolle — Sun, 14 May 2023 14:43:55 GMT

Sorry, but it's not working

Re: Reference dimension

dimamazutaMMJ32 — Sun, 14 May 2023 18:13:54 GMT

Hi @madstrolle! Try do use this iLogic rule.

Dim oDoc As Document oDoc = ThisApplication.ActiveDocument Dim oDim As Inventor.GeneralDimension Do oDim = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kDrawingDimensionFilter, "Select Dimension") If oDim Is Nothing Exit Do End If Dim oDrawingDims As DrawingDimension For Each oDrawingDims In oDoc.ActiveSheet.DrawingDimensions oDim.Tolerance.SetToReference Next Loop While oDim IsNot Nothing

(view in My Videos)

Re: Reference dimension

madstrolle — Sun, 14 May 2023 19:02:48 GMT

Not automatic, but it definitely works great, thanks 🙂

Re: Reference dimension

dimamazutaMMJ32 — Sun, 14 May 2023 19:10:11 GMT

Some input information is required to automatically changed specific dimensions. I thought that it is most appropriate to choose the sizes that should be reference dimensions.
If You need to change all dimensions then try this rule

Dim oDoc As Document oDoc = ThisApplication.ActiveDocument Dim oDim As Inventor.GeneralDimension Dim oDrawingDims As DrawingDimension For Each oDrawingDims In oDoc.ActiveSheet.DrawingDimensions oDrawingDims.Tolerance.SetToReference Next

Re: Reference dimension

madstrolle — Mon, 15 May 2023 06:01:42 GMT

I will try it 🙂

But it would be great if it could be done on the actually part. So every time I place the part and call for the dimensions they are with (reference). I'm using ilogic to generate these hole profiles.

I hope it makes sence.

Re: Reference dimension

dimamazutaMMJ32 — Mon, 15 May 2023 06:31:07 GMT

Please have a look at the standard Inventor command.
However, be careful, for this, the dimensions in the model must be reference, which can lead to accidental changes in these dimensions. A solution may be to impose a lock in the sketch's constrain. Then the dimensions will be references and the lines will not move anywhere. Please check the short video.

(view in My Videos)

Re: Reference dimension

madstrolle — Mon, 15 May 2023 10:15:34 GMT

But then I can't use ilogic to change the dimensions.

Re: Reference dimension

dimamazutaMMJ32 — Mon, 15 May 2023 10:44:34 GMT

The error occurs because the sketch geometry is locked.

In this case, there is no way to distinguish the normal size from the reference dimensions. If you have two types of dimensions in your drawing, then:
- If most of the dimensions are referenced, use rule 2 and then manually change the necessary sizes to normal dimensions.
- If most dimensions are normal, then use rule 1 and select those dimensions that should be reference.

Re: Reference dimension

dimamazutaMMJ32 — Mon, 15 May 2023 11:11:29 GMT

There is another way if you work with the templates of these profiles and you can add referenced dimensions to them. But these new additional dimensiones must be linked to another geometry.

(view in My Videos)

Re: Reference dimension

madstrolle — Mon, 15 May 2023 11:45:33 GMT

Thank you.

Together with the rule, this is perfect.

Re: Reference dimension

madstrolle — Wed, 27 Sep 2023 07:32:59 GMT

Hi @dimamazutaMMJ32 ,

I'm using this rule all the time, it's working great😊

Would it be possible to change the code, so it also works for "Ordinate Set"?