Documenting frame sketches

[skyeg3]

I have created a frame using the frame generator that I need to document. It is created using about 5 sketches. The sketches are part of their own .ipt file. Now I would like to document the frame but cannot figure out how to do it. I have tried creating sections of the frame but I cannot snap to points of interest on the frame, such as where two pipes meet, when dimensioning. How do I document the sketches?

Thank you,

Skye

[cbenner]

Hi and welcome.

You should have no problem creating a drawing of the frame, if you use the frame assembly as your base model for the drawing.  You talk about documenting the sketches, that's not really what you want to do.  The sketches are just the skeleton of your assemled frame.  Use the top level assembly as your base view and cut your section views from that.

If you are doing this and it is still not working for some reason, post your files here.  Also please let us know what version of the software you are using.  Have you been working with Inventor long?

[skyeg3]

The solution: Create a sketch on the view. Then dimension the lines that were drawn. Sketches can even be constrained to the view.

[cbenner]

This sounds like you are doing an end around for something that should not even be an issue.  Can you post some screen shots of the problem you were having?  One should never have to add sketches to a model view and then dimension the sketch. 

[skyeg3]

There are screenahots in the original message.  Here is another showing what I came up with.

[jeanchile]

When I do things similar to the type of frame you have, I use the Automatic Centerline tool for the view and then just dimension the centerlines. Did you try that?

[skyeg3]

I did but I wanted the centerlines to extend to point like in the screenshot above. I also wanted the centerlines for the curved sections of pipe which I couldnt seem to get with the centerline tool.

[jeanchile]

I'm on my phone and in a meeting so it's difficult to elaborate, but you can do everything you are stating with center lines and the dimension tool. If I get time later perhaps I can provide more but if you investigate the tools and help you should be able to get what you need. Good luck

[skyeg3]

Ok thanks, I will try again.

[jeanchile · Accepted solution]

Okay, now that I'm back at the office.....

I use the automated centerline tool to place all the centerlines for the cylidrical objects in the view:

With the settings to add centerlines to cylidrical objects:

That adds most of the centerlines. Then I use the centerline bisector tool:

To add the ones that are curved:

Then I just dimension to the intersection of the centerlines where I don't have orthagonal lines:

The centerlines are "extended" automatically by the dimension tool to show the graphic intersection. This dimension tool is where AD could really improve functionality because right now you have to select a line, right click, choose intersection, select the other line, the select another line, right click, then choose intersection, then select the other line which in and of itself is a cumbersome piece of crap but the really cool thing is that if you mis-click AT ALL you are rewarded by having to start the whole process over again! Thank you for that one AD. I only do this 1,000 times on every structural platform I create.

I also don't recall what happens when the pipes aren't normal to the drawing view (you have some like that) but I think you have to use the bisector for that too, I don't remember.

Hope this helps more than my previous posts. Good luck.

[skyeg3]

The centerline bisector is the trick I needed thank you.  I dont have an intersection option when I right click on a line though. My right click menu is shown here. I am using 2012.

[jeanchile · Accepted solution]

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@skyeg3 wrote:

I dont have an intersection option when I right click on a line though.....

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That's because you need to be "in" the dimension command. Start the general dimension tool, select a line, then right click. You should see this:

After you select "Intersection" when you move over to the other line you should see this:

Then you have to go through the selection process again for the intersection at the other end if there is one.

Good Luck.