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Wrong value displayed in drawing.

16 REPLIES 16
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Message 1 of 17
K.Luge
1136 Views, 16 Replies

Wrong value displayed in drawing.

See the jpeg:  1.345 is a regular dimension, .875 is a hole note.   The hole note is wrong.  Has anyone else seen this before?

 

(Luckily, the part doesn’t have to be scrapped.  It can be dissassembled, sent back for rework, refinished and reassembled.)

 

16 REPLIES 16
Message 2 of 17
JDMather
in reply to: K.Luge

I suspect there is a reason for the "wrong" dimension.

Can you attach the part and drawing here.

Finding the reason could save a lot of money in the future.


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Message 3 of 17
K.Luge
in reply to: JDMather

OK.  I've stripped the part model down to the offending features.

 

The wrong value is a cross port that intersects the larger hole (which is actually an ifeature).   Regardless of the intersection, or that the model was created 4 years ago, or that the ifeature was created in the dark ages - the only valid reason for a 1.35" diameter circle being assigned the wrong value is a bug.

 

It makes me wonder if the cross port will 'lend' its value to other intersected features.

Message 4 of 17
ampster402
in reply to: K.Luge

version of these stripped down models?  2011 cannot open them.

 

What version were they 4 yrs ago?

 

Were the 4 year old files ever migrated up to the latest version you are using?

 

newer_version.png

Message 5 of 17
K.Luge
in reply to: ampster402

"Version of these stripped down models?"

 

Sorry, I should've included that they've been saved under:       2013, SP1.1, Update 1, 64-bit

Message 6 of 17
JDMather
in reply to: ampster402

Inventor 8 last saved in Inventor 2013 - the reason you are getting that error in 2011.


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Message 7 of 17
ampster402
in reply to: JDMather

Yeap, saved in 2013 (or at least newer than 2011), figured that one out JD!

 

OP, without being able to see the actual Inventor 8 files, one guess I have is that if the files were never migrated from Inv 8 to a newer version and then just placed into an idw and saved, you might have found where the bug came into play.

 

 

Message 8 of 17
LT.Rusty
in reply to: ampster402

Has nothing to do with 2008-2013 issues.  The problem is that you're using a hole note on something that was not created as a hole feature ... but has an actual hole feature intruding on it.  The .75 diameter hole note on the 1.35 diameter hole is coming from the port drilled through the side.  If you suppress HOLE123, you'll find that you can't select the 1.35 arc with the hole note tool ... because it wasn't created using a hole feature.

 

It's more work to manually create the dimension you need in this case, but unless your hole was created using the hole feature, you can get some unpredictable results from using hole notes.  Sometimes it'll work okay, sometimes it gives you results like this.

Rusty

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Message 9 of 17
K.Luge
in reply to: LT.Rusty

Yes.  The problem of hole note vs. regularly dimension was already known – in fact, you don’t need to suppress the hole,  just make its diameter small enough that it doesn’t intersect that arc.  Also,  the problem of the cross ported hole ‘lending’ its value to surrounding geometry is, as you say, unpredictable (which is exactly what you don’t want from a cad program).  

 

The real problem - that Autodesk needs to fix - is the ability of the software to put the wrong value on geometry.    It is absolutely impractical to interrogate every dimension on every drawing.  That’s also why manually entering dimensions is bad, bad, bad and should be avoided. 

Message 10 of 17
LT.Rusty
in reply to: K.Luge

Why would you manually enter a dimension for this?  Just pull your normal dimension off that arc, right click on it (before setting it down) and tell it to be a diameter vice a radius.  Use the normal dimension tool, not the hole note.  That's what I meant by manual.

 

Autodesk will never be able to completely predict every possible interaction between geometry, and sometimes you'll get odd interactions between features like this where the software will get a little confused. There's higher priority things for them to worry about fixing. 🙂

 

The unpredictability I was talking about comes into play when you use the hole note tool to dimension things that were not created with a hole feature.  Sometimes a circular extrusion will be recognized as a hole, sometimes it won't - that's the part you can't predict.

 

 

Rusty

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Message 11 of 17
K.Luge
in reply to: LT.Rusty

 

...and  *manually* enter the hole depth.  (And no, a section view or break out is not an option.)

 

But seriously – forget the hole note thing -  if the value shown for geometry is unpredictable – what use is the cad?

Message 12 of 17
LT.Rusty
in reply to: K.Luge

You've got a lot more going on there than just a simple hole.  If you're going to document the geometry created by that iFeature, one simple hole note is probably not enough, and yeah, sorry, but a section view is going to be required.  That feature has 10 different diameters at various depths, 3 (I think) chamfers, threads, 12 different depths, counting the start plane and the point at the bottom.  A simple 1.35 x 4.xx deep isn't going to cover it.

 

A hole note is only going to reliably work when you're using it to document a hole feature.  An extrusion or revolved feature may or may not get picked up by it.  To put it a different way, there's some circumstances when you could use a crescent wrench as a prybar, but you shouldn't complain because it won't work as a prybar in every circumstance.  That's not what it was designed to do.

Rusty

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Message 13 of 17
K.Luge
in reply to: LT.Rusty

This is getting silly.  

 

With a threaded hole, one doesn’t need to describe the thread geometry, one can say ¼-20 blah-blah etc, and be done with it.  Same goes for various other things - JIC ports, as an example.  That part has a similar feature.

 

But seriously – forget the hole note thing -  if the value shown for geometry is unpredictable – what use is the cad?

Message 14 of 17
LT.Rusty
in reply to: K.Luge

If your crescent wrench's performance as a prybar is unpredictable, what use is your crescent wrench?

 

Use the right tool for the right job, and your results will be predictable.  Use the hole note tool on a hole feature, use the dimension tool on something that is not a hole feature.  Predictable - and correct - results every time.

Rusty

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Message 15 of 17
ampster402
in reply to: K.Luge

I don't see this as silly at all.

 

If the software wasn't designed to do what you want it to do, then either deal with the outcome of what happens when you try to use the software in that fashion, or change your methods to match what the software can do.

Message 16 of 17
K.Luge
in reply to: ampster402

 

But there are 2 holes there.   Both are about 4” deep.  So you use the hole note to find the one that’s about 4” deep and then you end up with the wrong value for the diameter.   But you’re not aware of this, nor are you aware of the fact that Inventor will show the diameter from a different hole,  and so you’re not predisposed to verifying that both dimensions produced by a hole note are correct.

 

So the assembly folks build the thing and it doesn’t work – they ask you why and you investigate and eventually discover that what looks like very legitimate dimension is wrong.  I mean, it’s not like tagging the quadrant of circle instead of the center.  You’ve got a leader pointing at a circle and a real dimension that looks to be correct except that it’s not. 

 

It’s silly that a cad program will put a leader on a circle and show the diameter of a different circle that’s in a different view.  

Message 17 of 17
karthur1
in reply to: K.Luge

Can't say that I have.  It looks like the hole was made with an ifeature.  Can you post this file too?

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