Drawing Dimensions not same as Part

[danwilley]

Hello,
I am working on a drawing and some dimensions are off by .0012 (inch) from the part. I have attached a screenshot of both the part (a simple revolution) and the associated drawing. On both screenshots, I have circled the dimensions in question in corresponding colors for clarity. Both dimensions are similar in that they are some count of 1/8" (.125). Both are incorrect by .0012". I changed the precision of both the part and drawing to 4 decimal places and that didn't fix the drawing. I made the part and drawing back in February of this year on the previous version and this problem was there too. I am currently on V21 and the problem still exists. I am in the process of adding tolerances to the drawing (ironically) and need to get past this drawing error somehow. Any thoughts and comments are appreciated.

Thanks,
Dan

 

[HaroldL]

Make sure the part sketch is FULLY constrained and the dimensions are to an axis. It appears the dimensions may be referencing a construction line that may not be constrained to an axis.
I would dimension to the Origin instead of an axis and use the axis only to create the revolve.

Select a point on the part sketch and see if you can drag it.
I've seen this before on some of my models.
Here's a quick test part I made up and the dims match part-to-drawing.

 

[DavidJ]

Please provide a package created from the drawing. In almost all cases there's a simple explanation for such apparent issues.

 

[oldfox]

What I see a lot of times is that when a sketch won't fully "auto dimension", it turns out to be a '0' (zero) dimension of a reference line
to it's parallel (actually on top of it) axis. I make this dimension manually and the sketch snaps into "fully defined". I think I will coin fixing
that little happening as "easter-egging".

 

[HaroldL]

When you dimension a sketch to an axis there is a reference line automajically projected from the axis to the sketch. I have found that sometimes that reference line loses its mate to the axis. If a new dimension is applied and uses that reference line to locate the sketch then both dimensions, the original and the new one, can be moved. If all dimensions for a revolve profile are dimensioned from an axis then each dimension will have its own projected reference line. That can be quite confusing if trying to trouble shoot a sketch that goes wonky. And that is why I have started to dimension to the Origin instead of an axis, though that may not be possible in all scenarios.

If I delete a dimension that referenced an axis then I try to make it a point to delete its projected reference line. When it is selected for deletion a warning pops up that it was automatically created to assist in constraining the sketch and recommends that you verify that it is okay to delete it.

The key point though is to make sure that the sketch is fully constrained no matter how it is dimensioned.

 

[oldfox]

The key point though is to make sure that the sketch is fully constrained no matter how it is dimensioned.

+100

 

[danwilley]

DavidJ... Here is the package.
Dan

 

[simonb65]

If you zoom right in on the sketch, you can see the reference line is not colinear with the revolve axis ...

 

[simonb65]

... constrain it, then save, re-project your views in the drawing and the dims now look good ...

 

[danwilley]

Harold,
I downloaded your testRevolve.AD_prt and see that you moved the part to the Origin and all the dimensions are correct. Given the "Scissor Arm Roller" part in the package, I just uploaded (see above), what is the best way to fix the part? How do I move the part to the Origin and establish a reference axis since it is currently based on a random parallel construction line?

(I am a relatively new Alibre user and still learning. This roller was the second part I modeled after buying AD Expert last February to experiment with the revolve function. I just made a construction line to revolve around. I did not know the importance of referencing parts off of axis, etc. )

Thanks,
Dan

 

[danwilley]

Simon,

Ok great, that was it. I zoomed all the way in and dragged the construction line down to the axis line. I tried to collinear constrain the construction line but couldn't pick the (axis) after first choosing the construction line. So I just dragged the construction line down to the axis line (zoomed all the way in) and that fixed it. The drawing is now correct. Not sure why I couldn't use the constraint function... my user error for sure. Also, not sure if what I did (dragging the line rather than a proper constraint) was just lucky and it may come back to bite me.

Thanks to everyone that replied.


EDIT: I went back and was able to do a proper collinear constraint. All is well now. Thanks again!

Dan

 

[HaroldL]

Dan, Looks like you found a solution. That's what I thought was going on, the reference line wasn't ON (collinear) to the axis. I've seen it several times myself.

Except for parts that you create using a Top Down method, Always start creating the part sketches on the Origin and aligned to the default planes or any planes you create referencing the default planes. That will also make it easier to place the part in an assembly using its default planes. What your are seeing with the reference line is one reason why I suggest dimensioning to the origin.

 

[danwilley]

Thanks Harold.

Yes, I modeled this part early in my Alibre (and 3D modeling) learning curve not knowing any better and have since started parts anchored at the origin or known axis' per several strong suggestions on the forum... probably some from you on other discussion threads. It just didn't occur to me that not doing so would create such a problem. When I created the revolve based around the construction line, Alibre behaved so normally it seemed. I selected the construction line in the revolve window, rotated the sketch, and all looked good. Who would have known there were these tiny dimensional errors. I kind of feel Alibre should have provided feedback or warning... or maybe even not manifested this dimensional error. (Seems like a defect to me.) Seeing the offset error as pointed out by Simon and your suggestion about fully constraining I now know what that means... ie: constraining the part to one of the "system" defined references... "Origin" in this case.. probably other solutions would work too. This experience drives home the importance of constraint, part reference "hygiene" and proper (Alibre) workflow .

Thanks again to you, Simon, et al for helping me understand and getting beyond this problem.

Dan

 

[NateLiquidGravity]

When I created the revolve based around the construction line, Alibre behaved so normally it seemed. I selected the construction line in the revolve window, rotated the sketch, and all looked good.

Check again. Being they were so close you thought you picked the reference line but accidentally selected the X-Axis instead. I don't think you can pick reference lines but you can pick regular sketch lines.

 

[JST]

....... I don't think you can pick reference lines but you can pick regular sketch lines.......
.

That seems to be true. Sometimes you can pick a ref line, other times you cannot. It seems to depend on the exact task you are doing that you want to use the "reference" line as a "reference" for.

Confusing, sometimes.

 

[NateLiquidGravity]

Yeah to further confuse: I converted the reference line to a regular line - that I could select for the revolve - and the revolve was created but failed because of an open sketch - so I edited the sketch (that was now attached to the revolve) and converted that line back to a reference line. AND IT WORKS!!! It even updated to changes in the sketch!

 

[oldfox]

I kind of feel Alibre should have provided feedback or warning... or maybe even not manifested this dimensional error. (Seems like a defect to me.)

I think your computer would have to become self-aware and tell Alibre what you intended to do after it read your mind. How else could it
(Alibre) know what you wanted. On the axis or not?

 

[DavidJ]

Dan - when applying constraint, first click the item that shouldn't move, next click the item that should move . So in this case, select co-linear tool, click axis, then click reference line.

 

[danwilley]

I went back and loaded the package I posted here into a sandbox to investigate further...

Nate... "Check again. Being they were so close you thought you picked the reference line but accidentally selected the X-Axis instead. I don't think you can pick reference lines but you can pick regular sketch lines."

Yes, that is what I did, selected the close-by x-axis as you pointed out. The x-axis and reference line were too close to see normally on the glass, and I thought the reference line could be used to revolve around. Apparently not, so Alibre chose what made sense to it (x-axis). I should have noticed that in the Revolve pop-up dialog.


David... thanks for the reminder of selecting the stationary reference first followed by the item to move. That worked immediately. I have read that before on this forum but in haste reversed the order. The school of hard knocks tends to drive things home.

Thanks,
Dan

 

[HaroldL]

Not to beat this to death but only as a point of reference, IF you would have been able to select the reference line that you had dimensioned to the drawing dimensions would have been correct. That they were not correct is because Alibre used the axis to create the revolve.

Here the reference line is dimensioned .125" away from the axis:



And the resulting drawing has dimensions that are too large by .125":



Here, to simulate using the reference line for the revolve axis, I placed an axis on the sketch reference line to use as the revolve axis and left the sketch .125" off the default axis:



And the result in the drawing is correctly sized dimensionally although it is not positioned on the model axis: