Dimensional length value changes randomly

[Anonymous]

So I'm working on a project, only a few days into learning this software, but I have a very simple cyclinder that I cut a revolution around, and the vertical height of this cylinder keeps changing depending on what part of the project I have built.  It's only by .02 mm but I don't want my measurements on the drawing to be wrong.  Originally, the value is (and should be) 12.  I next selected the top of this cylinder as the sketch plane and extruded a cylinder on top of it.  This is when the value decreases to 11.976mm.  I've had one rollback where even the first value was 11.976, but rolling forward then back again corrected it to 12.  However I am unable to get this value to 12 whenever the cylinder is built on top.  I have redefined the sketch plane as on top of the first cylinder multiple times with no change.  Does anyone have any suggestions?  As a last resort, is it possible to modify the values shown on my drawing sheet?  I see that I can edit the text after the specified dimension, but I do not see how to delete/change the specified dimension.

Aside:  I wish offset extrusion existed in this program rather than offset plane > sketch > extrude.

[HughesTooling]

Can you upload the file, from the file menu select export set the type to f3d and check save to my computer.

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@Anonymous wrote:

Aside:  I wish offset extrusion existed in this program rather than offset plane > sketch > extrude.

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Can you give an example, do you mean start the extrusion above the sketch plane?

Thanks Mark.

[Anonymous]

I attached the part file, and by offset extrusion I meant sketching on a surface, offsetting a distance from that sketch and then extruding using that sketch, similar to Solidworks (my native modeling software).  I saw many posts requesting this from months back so I was just mentioning it again so that autodesk is aware it's still a feature at least some of us are missing.

[kris_berg · Accepted solution]

Hi @Anonymous,

Welcome to the forum.  On your question:

As a last resort, is it possible to modify the values shown on my drawing sheet?  I see that I can edit the text after the specified dimension, but I do not see how to delete/change the specified dimension.

I have prepared a Screencast for you demonstrating how to the dimension value in a drawing.  Note the Screencast has me pressing delete/backspace twice.  You only need to do that once.

Thank you,

Kris Berg

Fusion 360 Development

[HughesTooling]

Something odd there, I did away with the sketch and just extruded the face and you still get an error!.

Before Extrude.

After Extrude.

Mark

[jeff_strater]

I think (but I need to verify with the team that owns it) that this is a Measure problem, not a geometry problem.  Or else it is a math problem with selecting the two edges and measuring.  I think that those two are really exactly 12 mm apart.  If I select the sketch profile from sketch3, and the planar face on the bottom, it shows up as 12:

But, if you select the circular edges, I get the same result as you do.  Let me check with the geometry guys - it's definitely weird...

Jeff Strater (Fusion development)

[HughesTooling · Accepted solution]

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kevincpiper wrote:

Aside:  I wish offset extrusion existed in this program rather than offset plane > sketch > extrude.

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OK now you've explained what you're after have you looked at Extrude Two Sided and entering a negative size for the second distance.

Mark

[jeff_strater · Accepted solution]

OK, I think I figured it out.  in Sketch2, there are really two points that are very close to each other.  this is causing your Revolve to remove just a little too much material, affecting the measure distance.  Here is a screencast of my fix for it:

Measure now works correctly, and I also tested a drawing after the fix, and it correctly reports 12mm

Phew, that was going to bother me all weekend otherwise.

Jeff

[Anonymous]

Thank you for the explanation on changing annotation values, Kris.

[Anonymous]

Also, thank you Jeff for finding the error within my sketch.  That's odd it placed my points 0.002mm away from each other instead of coincident in the first place.  And thank you Mark for showing me how to create an offset extrusion within the program.