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.)
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.
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.
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?
Inventor 8 last saved in Inventor 2013 - the reason you are getting that error in 2011.
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.
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.
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.
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.
Log into access your profile, ask and answer questions, share ideas and more. Haven't signed up yet? Register
Start with some of our most frequented solutions to get help installing your software.