Chamfer Dimension incorrect

[Anonymous]

I have a part which has a 5mm chamfer added on an edge. The adjacent edges are also chamfers 1mm

When I attempt to annotate the chafer in the drawing, I get an icorrect dimension.

During the Edge Selection, only part of the Chamfer Line is selected.

(See Screencast)

How do I annotate the correct dimension using the Chamfer Note?

[blair]

Are you current on all the SP's and Updated for your version of Inventor.

Can you post the part here as well?

[Anonymous]

Yep, latest SP's etc.

Here you go.

[mdavis22569]

I know why ..but not sure how to fix it ... or if it can be in this view. It would be possible in a section 

The chamfer is broken up into 3 different sections ....  .04in .12in and another .04in or .2in total (5.08mm) 

I'm up to date on everything too and can repeat it 

[Anonymous]

Yep,

My take on it is, it's the small 1mm chamfer around the part that is breaking the 5mm chamfer into diferent segments.

The Chamfer command in the Drawing environment can't handle the different chamfers meeting in the view.

[mdavis22569]

Nope, I tried doing it a few different ways, changing the order of the chamfers put on .. location clicks for the chamfer ...and nothing.  Only way is I believe is the section option

Mike 

[Anonymous]

Thanks anyway Mike.

I've worked around the issue by overwriting the length in the Chamfer note, but that is not fixing the problem!

[mdavis22569]

agreed ...I'm not a fan of faking/overwriting dim's either.

Mike

[blair]

I agree, I'll escalate the issue and hope ADSK can come up with something.

[SBix26]

Unlike the Hole/Thread Note tool, the Chamfer Note tool seems to not actually make use of Chamfer feature data.  It works equally well (or poorly) no matter how the chamfer was actually created.  On your sample part, I suppressed the 5mm chamfer feature, then recreated it by an extrusion cut, and the chamfer note performed exactly as before.

By contrast, the Hole/Thread Note will not apply to anything that was not created with the Hole or Thread tools, but it then makes use of all the data from those features.

Sam B

Inventor Professional 2016 Update 2
Vault Basic 2016
Windows 7 Enterprise 64-bit, SP1

[mrattray]

If your worried about that chamfer getting changed someday down the road and your drawing not updating (you should be), you could name the parameters in your model that are creating the chamfer and reference them in your overridden chamfer note.

[Anonymous]

Just revisited the drawing.

Try dimensioning the 1mm All Round Chanfer ! 

[LT.Rusty]

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By contrast, the Hole/Thread Note will not apply to anything that was not created with the Hole or Thread tools, but it then makes use of all the data from those features.

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Not entirely true.

You can use a hole note with an extrusion, BUT (a) the extrusion must be a circle, and (b) it has to be on a plane.  If your extruded hole is on something non-planar (which makes the mouth of the hole not-round) then the hole note won't work very well, but if it's on a plane it will correctly pick up both the fact that it's a hole and the correct depth (or thru, if appropriate).

[SBix26]

I'm pretty sure that wasn't the case the last time I checked-- maybe as recently as version 6...

Sam B

Inventor Professional 2016 Update 2
Vault Basic 2016
Windows 7 Enterprise 64-bit, SP1

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LT.Rusty wrote: 

Not entirely true.

You can use a hole note with an extrusion, BUT (a) the extrusion must be a circle, and (b) it has to be on a plane.  If your extruded hole is on something non-planar (which makes the mouth of the hole not-round) then the hole note won't work very well, but if it's on a plane it will correctly pick up both the fact that it's a hole and the correct depth (or thru, if appropriate).

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[LT.Rusty]

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@sbixler wrote:

I'm pretty sure that wasn't the case the last time I checked-- maybe as recently as version 6...

Sam B

Inventor Professional 2016 Update 2
Vault Basic 2016
Windows 7 Enterprise 64-bit, SP1

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Minor change: 2016 apparently CAN recognize extruded holes starting on curved surfaces, so long as it's round when you're looking at it in the drawing view.  See the attached drawing.

Although -  and this is disturbing - it doesn't seem to work any differently with an actual hole than it does when using an extruded circle.  I seem to recall that I could resolve holes made with the hole tool no matter what the upper surface of the hole looked like - on the attached part, I can only use the hole note when the hole is viewed square on.

[tewindle]

This Chamfer "problem", issue, whatever you want to call it has plagued drawings for many releases. I have also tried numerous part modifications to work around the issue. Sure you can add yet another section somewhere on the part that may only capture one of the two chamfers, but that is a lot of ridiculous unproductive work for a chamfer note. The end result is also having to modify the annotation manually, which is one of the worst things to do to accurately have a drawing represent a part. I wish there was a fix on the horizon, but I doubt it.

[mcgyvr]

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@tewindle wrote:

This Chamfer "problem", issue, whatever you want to call it has plagued drawings for many releases. I have also tried numerous part modifications to work around the issue. Sure you can add yet another section somewhere on the part that may only capture one of the two chamfers, but that is a lot of ridiculous unproductive work for a chamfer note. The end result is also having to modify the annotation manually, which is one of the worst things to do to accurately have a drawing represent a part. I wish there was a fix on the horizon, but I doubt it.

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Yep.. They know its an issue.. Its just seems to be a very low priority item.. (aka may never be addressed)

[blandb]

I have ran into this before as well, due to the smaller chamfer. When placing the note, notice that it is highlighting the small segment only. I always either did what was mentioned before, using a different view, or just using a dim and placing the 5 x 5 cham instead of the note to by pass it. That way there is no human text overwriting happening.

[IgorMir]

You don't have to override the chamfer note. Just don't use it in this particular scenario. Use a leader text and in the text itself - link chamfer dimension from the model. That's how it was done prior introducing the Chamfer note tool.

The thing is - Chamfer Note is taking information from the geometry on the drawing - not the model. And in your case - there is a chamfer on chamfer situation. That's why the reading is incorrect in the note.

Cheers,

Igor.

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@Anonymous wrote:

Thanks anyway Mike.

I've worked around the issue by overwriting the length in the Chamfer note, but that is not fixing the problem!

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[tewindle]

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@IgorMir wrote:

Use a leader text and in the text itself - link chamfer dimension from the model.

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I like this idea. How do you find the dimension in the model if you are using the Chamfer command in the part file? I cannot find any link to it in the "model Paramaters" in the text window.