intersection point - sketch (parts)

[Anonymous]

Hi,

I'm trying to find out how to attach a dimension to an intersection point of two lines. Have a look at the attached img - I have indicated which lines intersect and which point I need.

I know how to dimension it while detailind a drawing but I don't know how to 'grab' it while dimensioning a sketch before revolving or extruding.

Can anyone help?

Thx

[Curtis_Waguespack · Accepted solution]

Hi tom.boh,

You can use the sketch Split tool in combination with the Construction Line tool to achieve this:

Start off with something like this (fully dimensioned and fully constrained of course)

Use the Split tool (found on the Modify of the Sketch tab)

Set one segment of the split line to be a construction line:

Place a Collinear sketch constraint on the two segments to get the sketch back to being fully constrained

This link might be of interest as well:

http://inventortrenches.blogspot.com/2011/03/inventor-101-simple-fully-constrained.html

I hope this helps.

Good luck with all of your Inventor pursuits,

Curtis

http://inventortrenches.blogspot.com/

[Anonymous]

Thanks Curtis - you've spent some time answering 🙂

I should have mentioned that I know a way around the problem using construction lines. I was hoping that Inventor has got a simple intersection selection tool, similar to the one in the drawing part of Inventor (select one line, right click second line, select 'intersection' and voila!)

It's a bit strange that such a tool is available while dimensioning a drawing, but not while dimensioning a sketch.

Oh well maybe in the 2012 version 🙂

Thank you for your help 🙂

[JDMather]

What is wrong with using construction lines?
If you don't want to use construction lines simply make the point coincident with the angled line as well as the horizontal line and dimension.

[Anonymous]

There is nothing wrong with intersection lines, apart from the fact that I need to draw them. If I do what you suggest I still need to apply constraints. It's not automated and quick - that's all.

I've mentioned in other posts that I'm a former solid Works user so I have ways of sketching that are very mych 'Solid works' like. In SW to get the intersection point I'd select two lines and that click point and that's it - no construction lines, no constraining. I was trying to get the same from Inventor and failed 🙂

And I'm not moaning at Inventor - I'm new to it and I simply need to find my way around it. Inventor has got a lot of great features that SW doesn't (and vice versa).

[Anonymous]

I'm a big fan of construction geometry because it helps capture design intent. My profiles are obvious and the construction geometry show relationships.  

I have fixed a lot of poorly designed parts over the years, and it is always a pain to dig into someone's model and figure out why they did something. I want to make it as easy as possible to see how a sketch was constructed so I can determine whether they actually planned the model or just threw things together. For example, I create construction lines rather than just apply horizontal and vertical constraints. Even if I end up using a hor/vert constraint on the construction line, which is unlikely, the relationship between the entities is much clearer.

LorenJ

[SBix26]

I agree 100%!  I've run into sketches where where horizontal and vertical constraints are used between points in order to make co-linear lines.  Those are really difficult to track down.

[JDMather]

ditto

I use more construction lines in parametric CAD since than any time since leaving the drawing board for electronic drafting.  Not so much because they are needed, but because they help illustrate the design intent for later editing.  Remember how the instructor used to tell the board drafters - "...don't erase your construction lines..."

OK, maybe you guys don't go back that far into the last century.

[acad-caveman]

Where is the dead horse icon when I need it ??????

Just sayin' that dimensions like those are a 2 click non-issue in AutoCAD.

Don't get me wrong, I started using construction lines more and more, often times - not unlike the drawing board style - just trace the profile with solid lines.

But in this case all he wants is dimension a model that's already properly created. He now has to create construction geometry, dimension it and then make sure it is properly blanked when plotting.

Just what exactly is wrong with an AutoCAD style "App-Int" snap option?

[JDMather]

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@acad-caveman wrote:

He now has to create construction geometry, dimension it and then make sure it is properly blanked when plotting.

Just what exactly is wrong with an AutoCAD style "App-Int" snap option?

---

Uhmmm, it does work like AutoCAD in idw as the OP stated - that is not the problem.  No construction lines needed in idw.  Nothing to "blank".  I think the OP was referring to ipt sketches.  Of course there has to be a point there for a parametric dimension.  I think the question is should Inventor create this point automatically sketch as in SWx.

EDIT

I'm not convinced that SWx does this either.  I have been trying to duplicate and cannot seem to get it done as described bu OP.  There is an option in SWx to display Virtual Sharps that can be dimensioned to in part sketch - but I don't think that applies in this case.  I'll wait for the OP to come back and show me I'm wrong about SWx.

[JDMather]

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@Anonymous wrote:

I've mentioned in other posts that I'm a former solid Works user so I have ways of sketching that are very mych 'Solid works' like. In SW to get the intersection point I'd select two lines and that click point and that's it - no construc

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I can't get this to work in SWx 2010.  Can you post screen shots?

EDIT

OK, I finally figured it out in SWx.  Click first line, hold Ctrl key click second line and then click the Sketch Point icon to add a sketch point at projected intersection.  Then dimension as usual.  So one way or another an enitity (sketch point) must be created to have something to dimension to.

This would be cool in Inventor too.

Hmmm, except that it doesn't save clicks in SWx or fewer than current Inventor method that I can figure?

[Anonymous]

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@Anonymous wrote:

Remember how the instructor used to tell the board drafters - "...don't erase your construction lines..."

OK, maybe you guys don't go back that far into the last century.

---

Now you have me feeling all nostalgic.  Ah, those were the days.

[acad-caveman]

JD

Umm...   Well. Excuse me while I crawl back under my rock.

Missed that part, but OTOH I've just learned something new about the apparent intersection points in IDW.

Sorry!!!!

[Anonymous]

Just got to work and started reading the forum (different time zone to yours guys)

JDMather is right - this method of getting the intersection point he mentioned, is exactly what I was after. Select two lines, click on the 'point' button and there it is. Inventor has to it when dimensioning a drawing - click on dimension tool, click on 1st line, right click on the second line, select 'intersection' and here it is - dimension attached to the intersection point. Now simply select another edge or point and you have a domension to the required 'point'.

And I can't produce any SW screenshots as I have already left my former employer and the new one only uses Inventor.

All I have is my memory 🙂

apart form construction lines, the same result can be achieved by, placing a point on the 1st line and making it coincident with the second line (see attached file). Now the dimension can be applied to the point and will 'drive' the angled line - just another way around that I have discovered.

[JimSteinmeyer]

In solid-doesn't-works you select the first line, hold control and select second line. now select point and Wallla you have a virtual sharp that you can dimension for your drawing. If I remember Pro-E was simular but the point application was easier to select than if SW. I am now fighting to figure out how to make sharps having only used Inventor for a month and would like something quick and easy here too.

[JDMather]

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@JimSteinmeyer wrote:

In solid-doesn't-works you select the first line, hold control and select second line. now select point

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Isn't that exactly what I wrote in response 11, edit?

For your second question you should start a new thread with example of where you need the virtual sharp.

[JimSteinmeyer]

JD,

Sorry, I was in a hurry and didn't see that the thread continued to a second page. And for the second question, I thought that was basically what the OP was looking for, maybe I am using the wrong term.  but then again, I did skim several of the posts as they seemed to be pointed more for sketches than drawings.

Jim

[Scott_Parker]

In part modeling to create the intersection point quickly, you can start the point command, RMB, select "Point Snaps" and then "Intersection".  You can then select the 2 lines.  The point is automatically constrained to the 2 lines.

Scott Parker

Autodesk