Does anyone knows how to dimension an angular cut on a profile without having to sketch an auxiliary line (sketch entity), as shown in the screen capture below?
David Almeida wrote: Does anyone knows how to dimension an angular cut on a profile without having to sketch an auxiliary line (sketch entity), as shown in the screen capture below? Thanks,David
David Almeida wrote:
From SWX 2015 on you can select a edge then a vertex.
It will look like this.
Select one of the arrows to place your dimension.
Hope this helps!
Tried, but the coordinates arrows don't show up.
This is a Dropbox link with a video I recorded: Dropbox - angular dimension in a structural member.avi
Don't know if it is perceivable, but I tried .
David Almeida wrote: Hi Tony. Tried, but the coordinates arrows don't show up.This is a Dropbox link with a video I recorded: Dropbox - angular dimension in a structural member.avi Don't know if it is perceivable, but I tried .
David Almeida wrote:
What version of Solidworks are you using?
Perhaps I have some items hidden?
2018 SOLIDWORKS Help - Creating Angular Dimensions Using an Imaginary Line
Are you following these steps?
Nice trick. Didn't know this one.
Unfortunately can make it to work just in sketches of a part file. Tried to do the same in a drawing file and it doesn't work.
David Almeida wrote: Nice trick. Didn't know this one.Unfortunately can make it to work just in sketches of a part file. Tried to do the same in a drawing file and it doesn't work.
Don't know why it won't work for you. The images I posted are from a drawing. It does work.
Use the "Chamfer" Dimension Tool
It's a possibility. Tested and it works, though, in my opinion, this type of annotation is more suitable for sheet metal chamfers.
Just a thought but why not this:
In 45° angular cuts it doesn't make a difference, I agree.
But in angular cuts of 30°, for example, you'd have a complementary angle of 60°. This wouldn't be the correct information to send to the workshop to cut a 50×5 equal edge angle profile in a circular cutting saw.
To place the annotation as I wanted, I had to add a reference segment to place the annotation afterwards and it works fine. Just wanted to know if there is a faster way to do it, or if it exists a command at all.
Nevertheless, I appreciate your support.
Tony`s way works! Select edge, bottom vertex, TIP of right blue vector.
Yes, it works. Move mouse to arrow part of the line.
Don't know if I'm doing something wrong, perhaps I am.
I don't manage to have the "crosshair" in a view from a body part when using the tip Tony taught me.
With the feature "smart dimensioning" active, I pick the highlighted edge and vertex and it only appears an icon of angle next to the cursor. Similar to this icon.
Below the screen capture of this step:
In other hand, if I sketch 2 segments and use Tony's tip, it works perfectly:
Thanks to everyone.
I have a clue why I'm not managing to execute the command.
I tried in another part and managed to place an angular dimension using the procedure. I believe it is due to the fact I'm selecting an edge and a vertex that don't belong to the same entity/segment. For me, that's the only reasonable explanation...
If you all have the curiosity, I've chosen to pack both part and drawing for you to try doing it in drawing sheet "REF.ª 1", for example.
Dropbox - Carrinho máquina carga.zip
Check this option
I'm on SW2015.
In my case, too, it works on sharp edges (square/rectangular sections) but doesn't work on round edges.
You're right, if I select the point at the end of the straight top edge it works, as the point belongs to the edge, but unfortunately is not much useful!
I too have the same problem. But I have a super easy work-around. Convert the edge then use the angle/dim tool again.
I hope this helps,
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