Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Transform, Rotate Program Only


cnc22
 Share

Recommended Posts

    Is there a way in X8 to transform rotate the program and not the coordinate system. What I am looking for is using a double vise and want to keep my datums always against the solid jaw and stop. In the front set of jaws XY zero would be the rear left and in the rear set of jaws XY zero would be the front right ( part rotated 180 degrees around Z ). Then all I need is to increment my offsets for the number of vises that I use. I know this can be done by copying and rotating geometry but that makes the file more confusing and prone to errors if a change comes up.

 

Thanks for the help.

Link to comment
Share on other sites

I've done this with transform by toolplane Including the origin,  But I had to do a post mod to get the desired output.

 

%
O1234(1234NV1300.NC)
G0G17G20G40G49G80G90
N33T9933(INSERTED MILL)
M6
G0G90G54X0. Y-.9S1910M3T9934
M08
G43H99Z1.575
M98P1003
G90G55
G17G68X0.Y0.R180.
G0G90G55X0. Y-.9
Z1.575
M98P1003
G69
M5
G0G91G30Z0.M9
M01
 
N34T9934(ENDMILL)
M6
G0G90G54X-.6375Y7.78S850M3T9931
G43H99Z1.564M8
M98P1004
G90G55
G17G68X0.Y0.R180.
G0G90G55X-.6375Y7.78
Z1.564
M98P1004
G69
M5
G0G91G30Z0.M9
M30
 
O1003(SUB FOR 102235 INSERTED ENDMILL)
Z1.564
G1 Z1.364 F35.0
Y0.
Y7.007
Y7.907
G0 Z1.564
X1.103Y8.84
G1Z1.2497
G41D99Y7.94
Y-.895
X-1.103
Y7.94
G40Y8.84
G0Z1.4497
X1.103
G1Z1.1243
G41D99Y7.94
Y-.895
X-1.103
Y7.94
G40Y8.84
G0Z1.3243
X1.103
G1Z.999
G41D99Y7.94
Y-.895
X-1.103
Y7.94
G40Y8.84
G0Z1.575
Z3.375
X-1.383Y3.
G0Z2.5
M99
 
O1004(SUB FOR 102236 ENDMILL)
X-.6375Y7.78
Z1.475
G1Z-.05F18.34
G41D99Y7.33
X-.5625
X.5625
G40X1.0125
G0Z1.089
Z1.475
X-.6375Y7.77
G1Z-.05
G41D99Y7.32
X-.5625
X.5625
G40X1.0125
G0Z1.089
X.708Y8.465
G1Z.989
G41D99Y7.94
Y-.125
G2X.333Y-.5R.375
G1X-.333
G2X-.708Y-.125R.375
G1Y7.94
G40Y8.465
G0Z1.089
Z3.375
M99
 

%  

Link to comment
Share on other sites

I have been there. Hopefully I am missing something. When I use rotate it essentially rotates the coordinate system and I get an, A180 rotation that puts XY zero on the rear left corner again when it increments the offset. See the attached a file. the code in the transform is the same as the first path except for the A180. The backplot looks correct. Trying to get this setup with my double vise.

 

 

Tmp.TXT

Link to comment
Share on other sites

I am setting a different offset if you look at the file. It's the A180 and the code being the same. Both paths are in Quadrant 4 ( +X, -Y ). It should be the first path in Quadrant 4( +X, -Y ) and transformed path in Quadrant 2 ( -x, +Y ) so I can keep my datum references on the solid jaw and the work stop. Craig-B seems to have a solution but I am trying to do this without a post mod. I hate any unnecessarray copied or extra geometry.

Link to comment
Share on other sites

Rotate WCS about the Z-Axis 180°.  Rename new WCS Second Position or whatever else you wanna name it.  Change the Work Offset # to 1, (this will give you the home G55).  Now copy all toolpath folders and change the ALL Planes on the new folders to whatever you named your new WCS.  This will give you a new rotated coordinate system defaulting with a new home position.

Link to comment
Share on other sites

I am setting a different offset if you look at the file. It's the A180 and the code being the same. Both paths are in Quadrant 4 ( +X, -Y ). It should be the first path in Quadrant 4( +X, -Y ) and transformed path in Quadrant 2 ( -x, +Y ) so I can keep my datum references on the solid jaw and the work stop. Craig-B seems to have a solution but I am trying to do this without a post mod. I hate any unnecessarray copied or extra geometry.

Myth is correct about this. Select a new WCS and rotate it 180 degrees. Try not to use copy. Copying WCS has some problems. Select your new WCS and C/T planes and set them as G55. Copy tool paths. Se;lect all new tool paths and Edit common parameters and select g55 for WCS and C/T planes.

 

HINT: Standardize your WCS naming. By doing this, if you use Vericut it makes it EXTREMELY easy to create and execute a Vericut template that automatically fills in and selects your WCS info. Great time saver ;)

ex...

OP1 G54

OP2 G55

OP3 G56

 

spaces are critical

Also, never use TOP, BOTTOM, RIGHT etc planes. Always create new WCS planes.

  • Like 1
Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...