Making SolidWorks views like I see a part on my CNC machine 1

[vonbugburg]

I have a problem with the default views in Solidworks: front view, top view, and right view. I would like to see the top view (plan view) as I would be looking down at a part on the table of a CNC machine. Looking down on X and Y,Z up.

Ok, I rename the views, and switch (update) the views in the view box (the one with the "stick" pin on it).

All is well at this point. However, if I add a relationship, IE. hor. or vert. they are wrong. Therefore, I have 2 out of 3 pieces of the puzzle ok, but now how do I fix the relationship problem?

I figure there are a lot of parts being CNC'ed, and it would be more easy to do this when we are designing rather than in Surfcam/Mastercam. Would anyone help walk me through this?

 

[Dennyd]

Would it work to design your part on the default front view as though it is actually your top view? This should keep your horizontal and vertical relationships.

- - -Dennyd

 

[rockguy]

I would orientate my part(while building it) so the default top plane was my top view. This would require a little forthought before modeling. I use SW for a more architectural type application and I have my model set up so the top view is the plan view. Again I just have to give my modeling practice a little thought before hand. If the names front, top and right plane are confusing you could rename them to plan or XZ or something that makes sense to you. Save the the revised names in a template and then it will be the same for every part.

By the way. Tell AL I said hi.

 

[Theophilus]

Open your default part template and change your plane names such that your default view is in the orientation of the axes you like. Save the part template.

Now when you build your parts you'll have a default view orientation built-in. That's all there is to it.

Happy designing!

Jeff Mowry
Industrial Designhaus, LLC

http://www.industrialdesignhaus.com

 

[APPENG]

Von,

If you want to maintain all of the relationships and things then consider this. Design all you want without regard to the Coordinate system. As the very last feature you can then use the "move/copy" feature (INSERT/FEATURES/MOVE/COPY)
then rotate the model to the correct orientation for the CNC machine.

You may also want to look into using a customer Coordinate system then when exporting the data out to the cam software, you can specify that coordinate system.

Either way will allow you the freedom to do whatever you want then at the end spec out how you want the part to be oriented.

Hope that helps

Regards,
Jon
jgbena@yahoo.com

 

[tstanley]

Thanks for the tip APPENG, I gave you a star. I've often been bothered by this problem. To add to it I tried what you suggested then made a separate configuration for machining. That way you can suppress the move/copy feature in the original part so that it stays in it's as drawn configuration and doesn't disturb where it may appear somewhere else,perhaps in an assembly somewhere. Now when you open it in Surfcam, both configurations come in as separate layers. Just turn off the layers that are not oriented correctly for the CNC machine.

Tom Stanley