Stepped Boring

[KCollins]

We on occasion Machine Engine Blocks. For both the cam and Crank tunnels we have to do a stepped boring cycle. Rapid to -0-, Bore down to -1", Rapid to -2", Bore to -3"....I havent found a way to accomplish this in mastercam yet. Its the one thing thats keeping me from being able to say Mastercam can do everything our old logic based system could do...anyone have any ideas? I'm currently running 9.1 but have X to install this week

[Finecut]

Ok , here's is a work around.

As you know , canned cycles wont do this without a lot of help.

So you can use manual entry and a text file.

For boring try something like this:

S300 MO3

G0 Z0

G1 Z-1 F2.0

GO Z-2.0

G1 Z-3.0

.

.

G1 X-.01(LIKE A SHIFT BORE)

G0 Z.1

X0.

.

.

 

Got the idea ?

Now save it as a text file and use manual entry to input the code into your program.

Your post has to be set up in the comment field so the code will come out as code and not a comment.

Manual entry has 2 outputs. Code or comments. 1005, or 1006. You have to check the box that the post is set up for. some posts are not set up right. Here is my comment field:

 

pcomment # Manual Entry - COMMENTS (on a block by itself) 1005,1006

if gcode=1005, pcomment1 # Manual Entry Comment - 1005 - Codes

if gcode=1006, pcomment2 # Manual Entry Comment - 1006 - Comments

if gcode=1007, pcomment3 # Define comment with output line

if gcode=1008, pcomment2 # Define NC parameter comment - Operation comments

 

pcomment1 # Manual Entry - Codes - Without brackets

scomm = ucase (scomm)

n, scomm

 

pcomment2 # Manual Entry - Comments - With brackets and sequence number

scomm = ucase (scomm)

n, "(", scomm, ")"

 

pcomment3 # Manual Entry - Comments - With brackets and without sequence number

scomm = ucase (scomm)

"(", scomm, ")"

 

ptoolcomment #Comment for tool

tnote = t

toffnote = tloffno

tlngnote = tlngno

"(", pstrtool, *tnote, *toffnote, *tlngnote, *tldia, ")", e

 

pstrtool #Comment for tool

if strtool <> sblank,

[

strtool = ucase(strtool)

*strtool, " "

]

 

Use a g81 drill cycle at your center point and move the manual entry info into the g81 routine, and make sure you delete the g81 and the g80 code.

 

Finecut

[chris m]

I think you could use a custom cycle and use the Miscellaneous Real values to put in your points; I haven't done this but it should be possible.

 

C

[Glenn Stephens. from CCCS]

Use a point toolpath and select the different XYZ points changing between rapid and feed.

[KCollins]

Thank you. The point toolpath was just what i needed!

 

Long live the forum