topic Drawing dimension is wrong from part dimensions in Inventor Forum

Drawing dimension is wrong from part dimensions

snappyjazz — Thu, 25 Jan 2024 22:07:05 GMT

I modeled a pipe with a cope. When I dimensioned the Pipe in a drawing the dimension(See top screenshot) came out wrong. When I double checked my part, it is accurate(See bottom screenshot). So why is the drawing dimension wrong?

regards,

Re: Drawing dimension is wrong from part dimensions

SBix26 — Fri, 26 Jan 2024 00:18:09 GMT

Right click on the drawing view and check the setting of 'General Dimension Type'. I suspect that yours is set to True rather than Projected. If the dimension end points are not at the same depth relative to the view plane, there will be a Z component that you can't see, but which will add to the 'True' dimension.

If this is the case, you will need to delete that dimension and place it again.

Sam B

Inventor Pro 2024.2 | Windows 11 Home 22H2

Re: Drawing dimension is wrong from part dimensions

johnsonshiue — Fri, 26 Jan 2024 00:47:55 GMT

Hi! Right-click on the drawing view -> General Dimension Type -> select "Projected." Please share the file here. The forum experts and I can help take a further look.

Many thanks!

Re: Drawing dimension is wrong from part dimensions

snappyjazz — Fri, 26 Jan 2024 15:10:13 GMT

@johnsonshiue

@SBix26

Thank you for responding. I checked the view's dimension type and it was set to projected. I have also attached the part and drawing file...

Re: Drawing dimension is wrong from part dimensions

SBix26 — Fri, 26 Jan 2024 17:52:47 GMT

I can verify your results. In Inventor 2022.5.2 I see the same thing in your files, and I see the same thing when I replicate it from scratch in new files created from my templates.

I know that there are some inaccuracies that occur in models and drawings due to rounding and units conversions, but they are normally found quite a few more decimal places further in. This one is enough to actually affect a super precise (lapped, for example) fabrication process.

For what it's worth, creating the same model and drawing in Inventor 2024.2 results in a dimension of 19.12500000.

Sam B

Inventor Pro 2024.2 | Windows 11 Home 22H2

Re: Drawing dimension is wrong from part dimensions

johnsonshiue — Mon, 29 Jan 2024 22:34:35 GMT

Hi! I think this is a spline to arc approximation issue. On 2022, it seems that the approximation uses a loose tolerance so that the spline edge is approximated with a radius that carries some decimal places. There is indeed a change in behavior in 2024 and later so that the dimension is more precise now. The same dimension created on 2024 reads 19.125".

Many thanks!

Re: Drawing dimension is wrong from part dimensions

snappyjazz — Mon, 29 Jan 2024 19:48:16 GMT

Hmm, interesting; but also a bummer. Thank you @SBix26 @johnsonshiue !