Can someone please tell me how to create the dimension shown in an idw? Thanks.
I hope you can find useful the video attached.
Kind regards,
Alessandro
You can put a horiz dimension from the 2 points and then right click on the dimension and select align to edge and pick the angled line.
Your right, I had confused that with the center line align to edge. Sorry.
Sounds like a good wish list item.
That's just brilliant! Sorry, I can't thank you for your effort. Your video is just a poor workaround to the problem existed in Inventor from the day one. What if you have to dimension more then one trace like that? You guys should hook up for a lunch with your friends at AutoCAD team and find out in details how Align UCS tool works in AutoCAD. Then introduce that very tool in Inventor drawing environment. That is a solution to the dimensioning problem discussed, not the auxiliary sketch workaround.
Best Regards,
Igor.
@alessandro.gasso wrote:I hope you can find useful the video attached.
Kind regards,
Alessandro
this one gets me as well.... i gues they have never worked on the shop floor.
my saw operator is always asking for "long point to long point"
Can you post the drawing?
Chris Benner
Inventor Tube & Pipe, Vault Professional
Cad Tips Tricks & Workarounds | Twitter | LinkedIn
Autodesk University Classes:
Going With The Flow with Inventor Tube and Pipe | Increasing The Volume with Inventor Tube and Pipe | Power of the Autodesk Community | Getting to Know You | Inventor Styles & Standards |Managing Properties with Vault Professional | Vault Configuration | Vault - What is it & Why Do I Need It? | A Little Less Talk - Tube & Pipe Demo | Change Orders & Revisions - Vault, Inventor & AutoCAD | Authoring & Publishing Custom Content
You can add workpoints in the part model, then bring these points into the drawing, align them to the desired edge and dimension between them. I find this neater than adding sketches to the drawing views as I have had instances where the sketches in the .idw don't update and the dimensions then become incorrect.
Still not as neat as an 'align to edge' option though.......
Regards
Martin
I have noticed that (at least in recent versions) you can use the "chain" dimension type (not chain set) to achieve this.
place the dimension by hitting chain -> click on the line parallel to the dimension to be placed -> place as an aligned dimension -> RMB create -> drag one end of the dimension out to the long end of the bevel.
Dimension remains aligned to the first selected line (unlike a general dimension that will become a point to point when dragged to bevel end)
See attached (pretty rough quality ) video)...
Drove me mad till I discovered it.
Cheers
Don’t know why I wound up with 2 videos, they'll both be the same.
it complained that the 1400k was too big then accepted the 1200 and posted both!
This is a great tip (or is that a workaround?!). However, you have to be careful- a dimension placed that way does not maintain its alignment to that edge, so a model change that causes the angle of the edge to change will make that dimension useless. No problem, if the change is big enough to notice; possibly a serious problem if it isn't.
Thank you all.
I discovered you can do the same thing as was in the video with a base line dimension, but you end up having to erase a few of the base line dimensions to leave the one you want. The key is where to hover your mouse before creating the dim.
Of course, I can do this in AutoCAD (surprisingly enough, also an Autodesk product) with a rotated dimension, and it doesn't require nearly as much hand-eye co-ordination. It's also documented in Acad.
Can't find what you're looking for? Ask the community or share your knowledge.