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?
Solved! Go to Solution.
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?
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.
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.
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.
Log into access your profile, ask and answer questions, share ideas and more. Haven't signed up yet? Register
Start with some of our most frequented solutions to get help installing your software.