how to dimension from a line to where two other lines intersect?

[Anonymous]

still learning inventor.  I would think that it would be simple to dimension from one line to where two other lines intersect.  or from where two lines intersect to where two others intersect.

I have a case where I need to dimension from a horizontal line (a centerline) vertically to where another centerline intersects the outside.  in pro it was easy.  inventor, not so, or for me its not easy.

please see the attachment.

[SBix26]

It's easy in Inventor, too!  With the Dimension tool active, click the line, then click one of the other lines, then right click and select Intersection, then click the other intersecting line.

Or, place the dimension to some convenient point close by; then drag one end and swipe over both of the intersecting lines and drop it at the point where they intersect.  I use this method more often than the previous one, as I think it's faster and less clicking involved.

Edit: I see in your image that you're trying to dimension to the intersection of a line and an arc.  Unfortunately, Inventor does not currently create intersection dimensions when arcs are involved.  I don't have time at the moment to look for it, but I created an Inventor Idea (wish) for this functionality a number of years ago-- please vote for it if you find it (or someone else posts the link).

Hope this helps,

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Sam B
Inventor Pro 2019.0.0 | Windows 7 SP1
LinkedIn

[TheCADWhisperer]

Place a Sketch Point at the intersection.

If you can't figure it out - attach your files here and I will create a video.

[Anonymous]

after talking to a co-worker that's close to how he said to do it.    not so good way of creating a dimension. 

really need to be able to pick object lines, hidden lines, centerlines etc as needed to create dimensions.  I tried the other way that was suggested but it would not give me a vertical dimension.  I was getting a intersection but not the one I was needing.

[hosford]

If you are lucky and the point on the arc / circle is a quadrant, then the dimension intersection modifier method works.

[johnsonshiue]

Hi! Here is an article explaining how to dimension to virtual intersection.

https://knowledge.autodesk.com/support/inventor-products/troubleshooting/caas/sfdcarticles/sfdcartic...

Many thanks!

[IgorMir · Accepted solution]

Guys, the question was how to create a vertical dimension using intersection between the ark and a straight line. Not to quadrant, not between two straight lines. The answer is - it is a painful exercise in Inventor. I have been thinking - maybe to create a sketch in the view, project some entities and use them for dimensioning. But really - it is just a gross workaround.

Cheers,

Igor.

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@johnsonshiue wrote:

Hi! Here is an article explaining how to dimension to virtual intersection.

https://knowledge.autodesk.com/support/inventor-products/troubleshooting/caas/sfdcarticles/sfdcartic...

Many thanks!

[SBix26]

Here's a link to the Idea I mentioned earlier: https://forums.autodesk.com/t5/inventor-ideas/drawings-dimension-to-apparent-intersections-with-arcs....  It only has 44 votes, so jump in there and add more, please!

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Sam B
Inventor Pro 2019.0.0 | Windows 7 SP1
LinkedIn

[Anonymous]

for now, until there is a "good way", sketching a line as needed to trick inventor in giving the dimension is the only way.  stuff like this makes me think that the people who write the programs don't use the product...lol

thanks for yall's input

[TheCADWhisperer]

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@Anonymouswrote:

for now, until there is a "good way", sketching a line

I would simply add a Sketch Point to the Projected intersection.

[karthur1]

1. Start the dimension command (D on the keyboard) or pick it on the ribbon.

2. pick your horizontal center line.

3. hover the mouse over the intersection of the hole centerline and the outside edge. Pick the little green dot.

4. click to place the dimension.

You can swap the order of 2 and 3.  The only difference this makes is to where it will place the dimension.  It places the dimension on the side you pick first.  I think It should place it where you pick last... but that's just me.

[IgorMir]

Thanks, karthur1.

I guess - my previous experience did blind me. 🙂 Hence, there was my response to the OP with the suggestion of the axillary sketch.

Cheers,

Igor.

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@karthur1 wrote:

1. Start the dimension command (D on the keyboard) or pick it on the ribbon.

2. pick your horizontal center line.

3. hover the mouse over the intersection of the hole centerline and the outside edge. Pick the little green dot.

4. click to place the dimension.

You can swap the order of 2 and 3.  The only difference this makes is to where it will place the dimension.  It places the dimension on the side you pick first.  I think It should place it where you pick last... but that's just me.

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[donald_songras]

This works terrific.  Especially the drag and click, it is the only way that works when you're dimensioning with with an ordinate set.