HOW TO SELECT THE INTERSECTION OF CENTERLINE AND A OBJECT LINE

[Anonymous]

I CAN NOT FIGURE OUT HOW TO CREATE A DIMENSION LIKE THIS!

CAN ANY ONE PLEASE HELP?

[Mark.Lancaster]

@Anonymous

May I ask how someone would measure that on the actual part?  In the end you most likely would have to create a sketch on the view and project some geometry.

[kelly.young · Accepted solution]

Hello @Anonymous the easiest way would be to:

• Create 2D Sketch
• Use Project Geometry to bring in lines you want to reference.
• Draw the lines from the center of the circle to the outer point you want to measure to
• Finish the sketch
• Set the dimension
• Edit the sketch
• Turn the lines to Construction
• Finish the sketch 

You can also Retrieve Model Dimensions if you have set that dimension in a consumed sketch. If the sketch is not used to create something (extrusion, cut, surface) it will not be retrievable. 

Please select the Accept as Solution button if a post solves your issue or answers your question.

[Anonymous]

once again i have the need to dimension to the intersection of a centerline and a object line.  why does inventor not give you the ability to create such a each dimension without having to sketch this, sketch that, project, da, da, da!

pro engineering, creo si by far leaps and bounds better than this program.  dont't get me wrong creo has it's moments but making drawing it def has inventor beat.  should be so simple.  pick dimension tab (have options from point, line, intersection etc.  choose what you need and "get ER done".!

i'll see how much luck fairs sketching unnecessary lines.

do you know if this has been turned into inventor as adding it to it's next update?  how do you suggest things to be added?

[Anonymous]

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@Anonymous wrote:

once again i have the need to dimension to the intersection of a centerline and a object line.  why does inventor not give you the ability to create such a each dimension without having to sketch this, sketch that, project, da, da, da!

pro engineering, creo si by far leaps and bounds better than this program.  dont't get me wrong creo has it's moments but making drawing it def has inventor beat.  should be so simple.  pick dimension tab (have options from point, line, intersection etc.  choose what you need and "get ER done".!

i'll see how much luck fairs sketching unnecessary lines.

do you know if this has been turned into inventor as adding it to it's next update?  how do you suggest things to be added?

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submit it to the ideas forum....who knows, it may be in the next version.

[kelly.young · Accepted solution]

@Anonymous the two ways I showed in the screencast by creating a Sketch and Projecting Geometry or Retrieving Dimensions are the only ways I know how to accomplish it currently. Both are pretty quick and parametrically reliable so not sure how often you have to use this type of dimension and the amount of time it is taking to setup.

To follow up with @Mark.Lancaster question, is this dimension used for inspection or drilling the holes? It seems like this would be difficult to locate.

If you post at Inventor ideas make sure to reply back here with the link for others to vote up.

Please select the Accept Solution button if a post solves your issue or answers your question.

[Anonymous]

The dimension would have been used for inspection for me since there is no way one can measure it in the shop.
I can't believe that inventor can not do that. Every computer program I have worked on (not that there was many, just two bravo draft and creo) was able perform that.
For 27 years I designed gear boxes, bases, reservoirs, lube systems and gear sets at Lufkin industry so from time to time to ensure our drawings were correct we needed a dimension like that just to check and double check our design was correct.
Having more dimensions than required on a drawing is always better than too few. Having those also helped our checkers in confirming our design.
Perhaps the programmers in inventor might feel like writing a code or two to allow users to be able to add dimensions like that.

Thanks for your response and for the video!

[Curtis_Waguespack · Accepted solution]

Hi @Anonymous 

I'm late to this post... (just browsing as I wait for something to install/connect in getting a new laptop up and running)... but thought I'd add this info in case it helps in the future.

Inventor has a solution to this, but it's a bit different than what you might be used to.

• In the model file click the Create workpoint button then right click and choose Loop Select (I like to have Repeat Command selected also)

• Select the outer loop of each hole to create work points

• In the drawing expand the view node in the browser and right click on the model node, then choose Include Work Features...

• Then dimension to the included work features... note that if extra points are brought in you can turned those off by selecting them in the model tree node of the drawing browser and right clicking.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[Anonymous]

Seems to me this also applies to the perhaps more common situation of dimensioning to the intersection of two centre-lines, as in, for example, the bracing of a Warren girder. Which is a problem in Inventor. But again, in that case too, I think Curtis's solution of creating an axis or work point in the model, as appropriate, is the best we have right now.