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Drawing position changing after assembly mod


New member
I have placed an assembly into a drawing. When I rotate a component in the assembly around the component which is grounded the whole assembly moves position on the drawing. This is very frustrating when I have additions drafted over the assembly. I understand using snapshots, etc.

The whole drafting is also shocking by the way.


Try orienting the drawing view with a datum plane, that doesn't move (eg: a plane in the assembly).

This should fix the rotation of the view.

The thing about Pro/Detail mode is that it's only meant for detailing - it's not too hot on drafting...

Although - once you get used to the 2D sketch tools, they're actually quite useful.

I would say - do as much work in the part mode as you can - this is where Pro/E excels.. Then just do small tweaks in Detail mode.


New member
Yeah, it sounds like your drawing view doesn't have good orientation references. A good practice is to orient your views using saved views or assembly-level datum planes (default datum planes preferably).

Like proed said, you should be using the drafting tools as little as possible.

Dave Martin

Torgon Industries

Nose Bleed

New member
Yup - the above advisorees are good! From now on out, model everything from the same initial view point. I've had the same issues, but it all changed when I started the model from front, top, or bottom as the initial starting point, so that all parts have the same front (or other) initial starting datum plane. Thus, they are all easier to place into the assembly. However, it's a cop-out when it comes to making assemblies...

By any chance, are you trying to place multiple assemblies in an animation?


New member
i've gotten over the orientation problem some time ago.. as dave said, it's wise to use as little drafting as possible in drawing mode.. if in some case that you need to insert draft entities, oreint the entities to the view so that they will move together with the view (just in case).. but it's still a screw up when you change the scale..


If you have an assembly that gets bigger and smaller on the drawing views (from opening, closing or whatever), the views can shift around on the paper (left, right, up, down).

To prevent this, set the origin of the view by choosing Modify View / Origin / On Item and then picking a stable reference point on the drawing view. This is sort of like putting a thumbtack through the model into the paper at that point.

-Brian Adkins