Unable to dimension sketch in .idw

[DanielCTurcotte]

Hi everyone!

One of our draftsmen came up with a problem that I can`t seem to solve.

For some unknown reason, when he try to dimension a sketch inputted in a view in particular, it won`t work.

And its just for this base view, all other view created on the same sheet don`t have that problem.

I'm guessing that it would be something in the assembly that's causing this, but what?

I know that it would be a lot more easier if I shared that assembly. But my company as a strict sharing policy.

But i can still show you what it looks like, see attached. On the left, this i the one that we cannot dimension.

On the right is whats its suppose to be the final results.

Is anyone had, to some degree, that problem? And what could be done to fix this?

Tank you

Sorry for my bad English  

[cbenner]

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@DanielCTurcotte wrote:

Hi everyone!

One of our draftsmen came up with a problem that I can`t seem to solve.

For some unknown reason, when he try to dimension a sketch inputted in a view in particular, it won`t work.

And its just for this base view, all other view created on the same sheet don`t have that problem.

I'm guessing that it would be something in the assembly that's causing this, but what?

I know that it would be a lot more easier if I shared that assembly. But my company as a strict sharing policy.

But i can still show you what it looks like, see attached. On the left, this i the one that we cannot dimension.

On the right is whats its suppose to be the final results.

Is anyone had, to some degree, that problem? And what could be done to fix this?

Tank you

Sorry for my bad English  

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Is this a sketch created in the drawing file, or is this an actual model view?  There is a difference.  For that matter, is he trying to dimension to a sketch from within the model?  your use of the word sketch may confuse the answer to this question.

I suspect that you mean this is a model view, and it could be that something is rotated just a tiny bit off of square in your view, making it hard for Inventor to grab the points you want to dimension to.

If possible, post the files here.

[DeerSpotter]

Really Easy to fix 🙂 

select view, create sketch, select project geometry, Select all the lines you cant dimension and exit out. 

We have this issue with a lot of tube and pipe runs. 

Good Luck! 

[DanielCTurcotte · Accepted solution]

Dear M. Teleguz,

I've tried your way before, but it didn't work out. i wasn't able to dimension any line that i projected.

That was my main problem. But by further testing, see attachment, i found out that for some reason inventor was

seeing that view as an iso. So what i did, is making a custom view by assuring myself that i'm seeing directly on my plate.

And made it so that the view that i'm looking at is the top view.  

By setting my ViewCube --> Set current view as --> top.

Tank you all for your quick responses

[mgrenier25]

Same issue here, I am trying to dimension the diameter of a circle inside a sketch created in an idw, not from model.

I get the diameter icon on the mouse cursor when i hover over it but no dimension show up when I click, the view is flat in the drawing so it is not an alignment issue.

I have another view from the same model right beside this one (in a different position though) and the dimensions on this one will show properly.

[bradeneuropeArthur]

can you share the Drawing view?

[johnsonshiue]

Hi! The issue you are seeing may not be the same as the original one. Your issue seems to be related to sketch dimension (drawing sketch). Such sketch geometry is not considered view geometry (except Draft View). The sketch geometry is more like a note or transparency on a drawing sheet.

Many thanks!

[DayGriffin5218]

Same exact issue. Frustrating.

[DayGriffin5218]

This bug has to do with splitting the part. See attached screenshot. I revolved this shape, added some holes, etc.

When I split the part, you'll see that the top half actually creates two edges as opposed to a half circle. You can see this edge highlighted in red. The other solid does not have this edge, it is a complete half circle. 

When I place this view in the drawing (flat, of course so the face should be circular), I can drag radii dimensions without issue. What I am looking for is a diameter annotation. So, I tried to create a sketch on the view, project the center point, superimpose a coincident circle to the line, exit the sketch, and drag a diameter dimension to the sketched circle but it won't allow it. The diameter symbol shows up when I hover over the line but it will not create the dimension when I click it. If I suppress the split in the model, there is no issue with creating the circle and adding the diameter.