Inventor 2017 drawing annotation question

conceptdevelopers · Mar 13, 2017

How do you dimension to an intersection in INV. 2017? I have been getting a lot of prints without models and I have to make flat patterns. When they dimensioned theirs they do it an intersection. When I make my models its very hard to double check them without being able to do that

Freds · Mar 13, 2017

Having a bit of trouble understanding your question, so hope this helps...

If you are in a drawing, then choose Dimension, then right mouse click to get intersection option and pick two edges to form the intersection point for first dimension point. Choose second reference edge or repeat the intersection process for second point to complete the dimension .

If you have a model, need to establish a point(s) to dimension from. Start sketch on surface and project edges that will form intersection. Pick Point tool, right click and choose Point Snap - Apparent Intersection; now click on projected edges and Point will be placed. Now dimension from edge to that point (or between points you have created).

Fred

Brandonisneat · Mar 13, 2017

conceptdevelopers said:
How do you dimension to an intersection in INV. 2017? I have been getting a lot of prints without models and I have to make flat patterns. When they dimensioned theirs they do it an intersection. When I make my models its very hard to double check them without being able to do that

Do you mean an "apparent" intersection? Intersections on my computer snap easily/obviously. If you want an apparent intersection, you'll have to make a sketch on the drawing view, include the geometry that you need and make connecting lines in order to find the intersection. Then exit from the sketch and dimension the sketch intersection. Or at least, that's how I know how to do it, perhaps there is a more efficient method.

Hope that helps. If not, post a screen shot of what you're trying to dimension...?

conceptdevelopers · Mar 16, 2017

well it took me awhile to get back to this problem but here I am finally. I have tried to follow what seemed to be good instructions and have had no success.
feeling really dense here for a guy whose been using the software for years. I have attached a pic of what I'm trying to do. the 2.307 dimension is not to the entersection, close but that doesn't count. I'm missing something. Somebody please school this old fart :willy_nilly:

Freds · Mar 16, 2017

Have attached a drawing made in Inventor 2017....see it this provides an answer:

1) Click on Dimension
2) Click on line A - you get a dimension, but just ignore.
3) Right click and click on Intersect
4) Click on line B - you now have the two lines that form the intersection hilighted
5) Click on line C - you now get a dimension from C to the intersection of A & B.

Fred

Freds · Mar 16, 2017

Realized I essentially dimensions the part backwards from what you wanted, so here is same part a second dimension added; same procedure as before but:

Dimension - click C - Right click for Intersect - click B (two lines for intersect now hilighted) - click A for dimension from CB intersect to A.

conceptdevelopers · Mar 16, 2017

Thank you very much

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