Hello
How to orient the attachment on a drawing, like in this image:
Do we need to change the orientation of the view?
Create a landmark? If so, how do you define standard views as the front view based on a coordinate system created by the "Insert > Reference Geometry" menu?
Hi .PL
Haha, I thought I'd do this easy in insert mode and then right-click rotation. But in fact it's the reference plane that is rotten!
Indeed, you will have to create new plans if you want to position yourself in relation to them. Or you can directly orient your room as you see fit.
Then you go to display => edit => Orientation
There you have a new window that opens on the screen. Select "new view" (a spotting scope with a small yellow star/firework on top). You fill in the name of your view => ok
And then when you insert your part into the MEP, all you have to do is select the name of the view you just created
I hope I understood your expectation
Edit:
Otherwise, if you don't want to create a new view. Put your roof in the position that interests you. You follow the same procedure. Except that instead of "new view" click on "update standard view" (a spyglass with rotation arrow). It should reset your views. But never tested, you'll tell me if it works well
Same as coin37coin,
I use the "update standard views" option which redefines your views from the current view and the view you want it to correspond to.
Otherwise, without modifying the views of your part, you can position yourself in the 3D with the orientation of your part you want and choose in the drawing to insert the "in progress" view
Coin37coin has given the right method for the general case and I confirm that the update of the standard views works well (by the way, be careful if a drawing has already been created, the views will follow...)
In this case, if it is possible compared to the rest of the project, the easiest way is to add a body displacement function (insert/function/move-copy) using the constraint method (cf pdf in attachment).
To tell the truth, I would also be interested to know if we can, and especially how, define a view by 2 planes.
Another solution that works well (especially since you have an imported part so we don't care about the loss of information, right?) is to use an assembly and re-save in sldprt format. You insert your part in it and constrain it in relation to the sub-assembly plans. I don't know if that's stefbeno's solution?
In any case it works for your piece (see attachment)
It's the fastest because I tried the method of redoing the views but it's not easy to have the right plan well oriented with your room (it requires patience...)
Hi .PL
I've already seen this piece somewhere:)
In fact, the quickest solution (in my opinion):
- You open the room
- You put yourself normal on the flat face that should appear on your drawing view
- You update the standard views to set the current view as the front view
- You create your drawing and you put your view
- You select the edge that should be horizontal on your plan view
- You go to Tools, Align Drawing View and you choose: Stop Horizontal, your view will be as defined in your image, the manipulation lasts about 30 seconds
I asked you a video
A+
Mick
Tip top with the latest @Mick manip! (too bad it's not in 3D this one by the way)
Hi .PL,
No existing improvement request to my knowledge
A+
Mick
Hello
I don't really see the difficulty, I must have missed a piece of information!
If you want to reorient your volume in relation to 2 sides, you have to select 2 sides during the "Normal to". The first will be FACE, the second ABOVE.
And then you update your views, or you save as a new view.
Edit: image redone.
Indeed, your solution is even simpler Benoit!
Thank you!
Ouoooh Benoit, hats off to the trick!
Indeed, it is even faster.
Bvo
Well, the trick with both plans. !