(T/C plane parameter) What's it supposed to do?

[nickelback]

What applications would you needto use the T/C plane parameter? I did some y/z contouring, more less cut a rainbow in the side view,using this T/C parameter. I would like to know what are the origins x,y,z for when you use this T/C plane option. And what kind of applications do you use this option for. I can't find anything in any books and it's driving me nuts!!

[Michael Reynolds]

I use the T/C plane option to set different work coordinate settings, like G55, G56, etc.

Hope this helps!

Mike R.

[Simtech]

The T/C plane option allows the programmer to set a new coordinate system in Mastercam for different purposes.

Cplane: with this option you can set a new origin for your coodinate system. The XYZ values that you will see in the T/C plane window are the coordinates of the 'transformed' plane from the world coordinate system. To set this new origin when in Mastercam, choose the Cplane menu in the secondary menu and then hit Alt-O for origin.

Tplane: exact same explanation for the toolplane.

Here's an example:

Lets say you draw a rectangle 6 X 4 with the origin set at the lower left corner. If you set the new Cplane origin to the upper right corner and analyze the lower left corner point, you will obtain (X-6, Y-4) because the new origin is shifted. (notice the star next to the T in the Cplane menu indicating the shift)

Hope this helps!

Luc

[d0gFartz]

Best to use your named views in conjunction with

that,then you could name each part by say it work

offset and just set it active to program the T

path

 

[Guest CNC Apps Guy 1]

Or you could be like me and have 1 part in your file a,d just access the different sides and set each T/C plane.

I despise having multiple files for the same part. Even My fixtures that I program are in the same file. There is just no real need for multiple files.

JMHO

[d0gFartz]

Hence the advantage of the named views,1 file

containing all your planes and offsets assigned

to your file

[bb]

Try this construct an axis like the one in the bottom left corner of the screen at x0 y0 z0.

change view to isometric.

change consruction plane to isometric.

cplane,next menu , = gview

construct a circle at 0,0,0

save this drawing into your patterns directory for latter use.

open a existing mc8 file

cplane

rotate

(rotate cplane axis )

save

cplane

next menu

save named

(name the view)

(set the origin)

ok

tplane

next menu

=cplane

 

create

next menu

pattern

name

(choose the axis you created previously)

do it

0,0,0

this places the axis relative to the construction view and origin

gview

entity

(pick the circle in the axis pattern)

this will give you an isometric view of the setup

hope thyis has been of help

[3d-machine]

It's for:

1)toolpathing the hole part within 1 file (good for verifieng purposes too hint i put an arc at my new tool plane points makes it easier to select as an entity and for referance).

2)doing rotary axis moves (mpfanuc.pst (post file) should cover most machines).

3)you can set these as different offsets g54,g55 atc.(good for multi-setups)