normal to

I ask my VAR how SWx was determining things like horizontal/vertical ect in reference to planes (essentially what you have when you select a planer surface). Basically he explained that there has been a long standing consensus among cad software companies ( might have started with the iges std ) that determines, based upon the origin of the plane and its relationship to the part/assemblies main coordinate system, how a plane gets oriented ( a long mathematical solution ). Unfortunately, although it would be much more user friendly to be able to toggle such things, SWx has no plans to deviate from said convention. If you are lucky, someone out there may have a macro that can help.

"Rudy Kazuti" wrote in message news: snipped-for-privacy@comcast.com...

I gave up trying to do this. Never works the way I want.

When sketching at some oddball angle, the first thing I do is lay down two perpendicular construction lines to use as a local coordinate system. Instead of using horizontal and vertical constraints, I use parallel/perpendicular to the construction lines. I found this to be an effective way to deal w/ odd-angled sketches, especially if the plane ever moves or flips.

Another thing I like to do is add base axes for X, Y, and Z right after the origin. That way I can pick them for parallel/perpendicular reference right off the feature tree.

One thing Pro/E did right was to allow users to pick horizontal or vertical references for sketches. Sketches updated according to references. Also handy was that you could pick which side of a plane to sketch on.

A very nice deviation from convention.

Here is a workaround: hold down shift and hit the arrow key to rotate anything 90 degrees at a time.

Stephen

Rudy Kazuti wrote:

just want to make it clearer. With the shift+arrow workaround, you need 3 clicks to switch between vertical and horizontal. Shift+up, left, down is one combination that will work.

clicklik

Rudy, Instead of single selection, make two selections. The first is the sketch plane, then while holding the "Ctrl" key, make a second selection and finally, "N" for normal. The second selection will face top or upward. If the view will be required again & again, save it as a named view. Eddie

Ok, thats a handy tip ( just used first time ). Now I have to use it often enough that it becomes part of my sw repetoire before forgetting about it.

To pick the view on a model you want to draw on, first pick the face you want your sketch on, then while holding the "ctrl" button, pick the face you want to be "pointing up", and press the "Normal To" button on your standard view toolbar.

The view always seems to swing anywhere it

In an assembly, the normal view of a part is dependent upon its top, front and right planes. Front plane will be vertical and the right plane horizontal to the screen

Kman