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Dimension to the intersection of 2 centerlines

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Message 1 of 25
ChadMH
2117 Views, 24 Replies

Dimension to the intersection of 2 centerlines

I need to dimension from the intersection of 2 centerlines to a hole.  Can anyone help?

24 REPLIES 24
Message 2 of 25
LT.Rusty
in reply to: ChadMH

In a model or in a drawing?

Rusty

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Message 3 of 25
Ryan.Martinez
in reply to: ChadMH

Post a screenshot or file.... something to help illustrate what you are trying to do.
P.D.S. 2015
P.D.S. 2016
Message 4 of 25
ChadMH
in reply to: Ryan.Martinez

it is the 2.841 dimension.  I faked it but still need to know how to do it.  Thanks for the help.

Message 5 of 25
LT.Rusty
in reply to: ChadMH

Create a sketch on the drawing view (hint: select the view BEFORE you hit the create sketch button!).  Once you've done this, use project geometry to get the inner and outer diameter of the flange that's drilled, and to get the hole that you're trying to dimension from.  Use the line and point tools to get something in the right place to anchor the dimension that's the intersection of your centerlines.  (You can't project the center lines, unfortunately.)  Once you have the point in the right place, finish the sketch and then set your dimension (make sure you right-click and set the dimension type to ALIGNED).  Go back afterwards and edit the sketch so that the line you used to locate your point is set to SKETCH ONLY.

 

It seems like cheating, but I think it's probably the only real way to get what you want.  It's not really cheating - your dimension will update if you make changes to the model, so long as your bolt pattern diameter maintains the same relationship to the center of the part.

Rusty

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Message 6 of 25
ChadMH
in reply to: LT.Rusty

That is basically what I did but I thought there was no way it was that complicated. That is really disappointing that Inventor cannot perform such a simple task. Anyway, enough venting.

Thanks for your quick, detailed and well explained response.
Message 7 of 25
LT.Rusty
in reply to: ChadMH


@ChadMH wrote:
That is basically what I did but I thought there was no way it was that complicated. That is really disappointing that Inventor cannot perform such a simple task. Anyway, enough venting.

Thanks for your quick, detailed and well explained response.

 

You're welcome.

 

In all fairness, this is not an issue that really crops up with much frequency, and the problem seems to be with the fact that your centerlines intersect at more than one location.  When you have two centerlines that are just straight lines you can pull intersection dimensions with no problem.  In this case, though, you've got a cross-shaped center mark and then you used the center line tool to create the circular array.  Because there's only effectively two center lines, which intersect in ... I think about 20 different places and ways, this makes Inventor get a little confused and it doesn't know which of the intersections you want to work with.

Rusty

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Message 8 of 25
Ryan.Martinez
in reply to: LT.Rusty

Start the dim tool - select the circle first - select the intersection of the center lines - right click during the placement of the dim and select aligned see my attached pdf... no dwg sketches there
P.D.S. 2015
P.D.S. 2016
Message 9 of 25
ChadMH
in reply to: Ryan.Martinez

I dont see a PDF.

 

Thanks

Message 10 of 25

Not sure why my pic won't post...
P.D.S. 2015
P.D.S. 2016
Message 11 of 25
ChadMH
in reply to: Ryan.Martinez

Doing what you described works except there is no option for "aligned" when I right click.  It will only let me dimension to the centerline, not get the chord dim I need.

Message 12 of 25
Ryan.Martinez
in reply to: ChadMH

should work if you click the circle first and then the center line intersection
P.D.S. 2015
P.D.S. 2016
Message 13 of 25
LT.Rusty
in reply to: Ryan.Martinez

Please demonstrate with the attached .IDW file.

 

I haven't been able to make your solution work either ...

Rusty

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Message 14 of 25
Ryan.Martinez
in reply to: LT.Rusty

I realize now that I was cheating. If you turn the visibility off on a hole while in an IDW you can still pick up the center point. Apologies, I tend to like to use model dimensions so another way to do it would be in the model while you are sketching the bolt circle. Isee the links below and sorry for the confusion. 1. http://s1252.photobucket.com/user/massatk/media/Step1_zps41934a35.jpg.html?filters[user]=140375035&f... 2. http://s1252.photobucket.com/user/massatk/media/step2_zpsb5c91443.png.html?filters[user]=140375035&f... 3. http://s1252.photobucket.com/user/massatk/media/step3_zps49502408.jpg.html?filters[user]=140375035&f...

P.D.S. 2015
P.D.S. 2016
Message 15 of 25
Adrian010
in reply to: LT.Rusty

I have a truss made off tubing and want to dimension to the intersection of 2-3 center lines of the diagonal braces, this is impossible.

I have tried the sketch method and it will not let me dimension aligned, this is terrible, I had to do a work around and its a Shi ty result.

 

Message 16 of 25
LT.Rusty
in reply to: Adrian010

Attach your files, let's take a look and see what we can do.

Rusty

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Message 17 of 25
Adrian010
in reply to: LT.Rusty

I cant attach my model, but you can replicate this your self, see attached screen shot.

What I want to do is either running dims or regular dims in series so the fabricator can just run his tape and mark out the nodes to layout his pipe.

I have messed with all the options and sketch. If you have a solution that would be great.

 

The one thing I noticed that retarded is you can dimension to the end of the center line, BUT you cant make the center line endpoint align with the other center lines with out any accuracy, this is frustrating the hell out of me..

Message 18 of 25
LT.Rusty
in reply to: Adrian010

Okay, that's easy, and you don't need the sketch trick for that.

 

 

Start the dimension tool and pick the first centerline.  Right click, select INTERSECTION, then pick the centerline that crosses it at the point from which you want to dimension.  Repeat this with the second set of intersecting centerlines, then right click again and under DIMENSION TYPE pick ALIGNED.

Rusty

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Message 19 of 25
Adrian010
in reply to: Adrian010

DUD Thanks Smiley Happy

Message 20 of 25
LT.Rusty
in reply to: Adrian010

And yeah, I feel your pain on the centerline length issue. That's an annoying one for sure. Maybe enter that one in the Inventor IdeaStation? I'd certainly be along quickly to give it an up-vote.

Rusty

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