Choosing the sketch axes in solidworks?? How? 2

[Baroche]

Hello all

in Solidedge, it is possible to specify/indicate the base axis for a "normal view" sketch.

How on earth do I do this in Solidworks. How do I control the orientation of the model when I enter the sketch environment?

Thanks for any help

 

[JMirisola]

Your initial sketch will determine the orientation of the model. Upon invoking the sketch command, it automatically goes 'normal to'. This only happens in the very first sketch. Subsequent sketches can be made normal to by hitting ctrl+7, or hitting the 'space' bar and selecting 'normal to', or you can choose it from the 'view' menu.

Jeff Mirisola, CSWP
Certified DriveWorks AE

http://designsmarter.typepad.com/jeffs_blog

Dell M90, Core2 Duo
4GB RAM
Nvidia 3500M

 

[Baroche]

Thanks for reply.


However once in the "Normal view" to the selected plane, is it possible to control the orientation of the model. In SE you can control the orientation of the model in the Normal view by indicating the base axis for the sketch. You do this by selecting an edge or plane on the model as the direction of the base axis.

In Solidworks I am having to rotate the sketch because the orientation of my model is not ideal (even though it is normal)

Any similar function in Solidworks? I'm using 2008.

Thanks

 

[TheTick]

When doing models at odd angles, I've developed a habit of not using horizontal or vertical constraints at all. I make two construction lines that act as a coordinate system and constrain parallel or perpendicular to those, instead.

Pro/E also had nice functionality that allowed one to determine sketch orientation. With all of the pseudo-improvements SW has made, this is not one.

 

[mjcole]

This is actually a good thing I like about SW is that it doesn't demand orientation set up and thus reduces the number of references for a sketch.

The easy way to orient your sketch is to sketch a point on the default sketch origin L and use the Modify Sketch tool. This will allow you to both move and rotate the sketch.

Don't worry about view direction because when you use the View Normal To (CTRL+8] it flips direction on each use. The sketch dimensions will be visable in the correct orientation all the time.

I believe the default orientations are based as follows when parallel to any of the default planes.
XY
YZ
ZX

I also highly agree with TheTick's observation and technique. You can create a construction line and make it collinear to an edge or axis.

If you have a sketch with a bunch of H and V constraints or Relations and you choose to place it at an angle you will have some good fun with Display/Delete relations or Dealing with the Diagnose Sketch tool which is great if you need it.

Michael