Need Help, part is in wrong spot

[ZipSnipe]

I,m using Mastercam x2, when I verify everything looks good, however when I post to my machine and then verify on its controller its reversed or when I try a few things such as mirror the part in Mastercam then the machine wants to start like its reversed. Any ideas?

[Superman]

Your selected WCS is incorrect.

set your WCS active, and view TOP.... this is your setup in the machine for all the operations

If you change the part orientation, then a new WCS is needed, with new C & T planes,
the new C & T plane orgins should be the same origin point as the WCS used

[ZipSnipe]

Thanx for the reply Supe, I change the WCS at the lower right hand side of the screen correct? where it says wcs?

Also can I set the wcs to the stock part position?

[Superman]

Thanx for the reply Supe, I change the WCS at the lower right hand side of the screen correct? where it says wcs?

Also can I set the wcs to the stock part position?

Lower toolbar is where you manage your views ( View Manager )
One of those views can be your WCS, which must be set in the "Planes" section of the toolpath operation. The T & C plane is the working plane of the spindle axis in relationship to the chosen WCS

for example
you have a block, sitting in space .say it is standing on one corner

-you can rotate your views to align this part as you would set it up in the machine, you then name the view and set an origin ( some may set the origin on a feature on the part ( bore, corner etc) or on a feature that is used to fixture the part ( dowel, boss, etc) .

-this is then used as the WCS for any operation in this setup

-if working from the TOP face only ( 3 axis machine ) the T & C planes will be the same as the WCS
-if you want to machine the front face, then a new view ( as seen by the tool spindle ) must be created and the origin must coincide with how you operate your machine's co-ordinate system.
- using the WCS and new "Front" view allows mastercam to output an A90. in the program for when using a 4th axis

the WCS & planes are set before creating the operation, or you can go into each individual operation and alter them in the "Planes" tab after the ops were created, ( advanced users could used the "modify common parameters" procedure )


(NOTE) it is good practice to create your views as seen from the tool aspect, this can eliminate the program being 180° out ( if you use the default BACK & BOTTOM views for a machine with a 4th axis anlog the X-axis)

[ZipSnipe]

Kool thanx Supe!! you truly are Superman!!! Excellent explanation!!!!

[ZipSnipe]

uummmm this is weird, it verifys correctly in mastercam, and it verifys in reverse on my controller but it's cutting the part correctly. Oh well!!

[Superman]

OK, ( it does sound a little weird ), but you have got it working....sort off

Just to check your settings

your "new WCS", plus C&T planes are set correctly in the operations ?

yuor "Stock setup" is using the "new WCS" ( stock is then defined in relation to this "new WCS" (---this sets up the verify session )

when you set the new WCS active with the C/T planes ( view manager, set all the same ) then go to view the TOP ( TOP view of the "new WCS" )

this should be how you have set the stock / part in the machine and your toolpaths are created to suit this arraingment

verify only shows the NCI file operation toolpaths, it is NOT displaying or verifing any NC code whatsoever.