Drilling cycle putting in 9999.

[medaq]

I know it is not common to use all the linking parameters to be of the same value. In most case you would be drill or doing something. But I have used this method for over a decade to position a tool and enter code like probing, back boring, special clearance moves for tight area with no clearance, or just using a pin for locating a quick part, or add special movements for undercut and clearing what I need.

 

I can make the program work by changing the z depth .0001 and all will be well. But I dont want to have to remember to do that for all of the programs I will do this to in the future. Is there any way to have mpmaster pst output the numbers correctly the way I put them into the linking parameters instead of adding in this 9999. in area of duplicate values?

 

%
O0000 (T)
(MPMASTER GENERIC 3/4-AXIS HORIZONTAL)
(HPLUS 300 PC15 OP1)
(MCX FILE  - Z:\MASTERCAM\PRODUCTION\A.....)
(PROGRAM   - T.NC)
(DATE      - APR-18-2017)
(TIME      - 9:10 AM)
(T106 - DEFINE TOOL NAMES    - H106 - D106 - D1.0000")
N100 G00 G17 G20 G40 G80 G90
N110 G91 G28 Z0.
N120 T106 M06 (DEFINE TOOL NAMES)
N130 (MAX - Z.1)
N140 (MIN - Z.1)
N150 G00 G17 G90 G54 X-.9649 Y-3.7203 S9000 M03
N160 G43 H106 Z.1
N170 G00 Z9999.
N180 G94
N190 G98 G82 Z.1 R9999. P2000. F50.
N200 G80
N210 M05
N220 G91 G28 Z0.
N230 G28 Y0.
N240 G90
N250 M30
%
 

[Colin Gilchrist]

The short answer is "Yes", of course there is a way. I don't won't be able to look until later this evening when I get home.

I just have to ask though; is this just a positioning move? Do you need the Drill Cycle (G81/G82 line)? 

I think you would be much better served by using a "Point" Tool path, and modifying the Canned Text function to output your Macro Call. Or whatever special codes you need. Much less headache that way, and you don't screw up the Drill Cycle logic.

Try it out. I think you'll be pleasantly surprised. If you are doing a "Pin Stop", I would absolutely advocate for using the Point Tool path.

[medaq]

9 minutes ago, Colin Gilchrist said:

The short answer is "Yes", of course there is a way. I don't won't be able to look until later this evening when I get home.

I just have to ask though; is this just a positioning move? Do you need the Drill Cycle (G81/G82 line)? 

I think you would be much better served by using a "Point" Tool path, and modifying the Canned Text function to output your Macro Call. Or whatever special codes you need. Much less headache that way, and you don't screw up the Drill Cycle logic.

Try it out. I think you'll be pleasantly surprised. If you are doing a "Pin Stop", I would absolutely advocate for using the Point Tool path.

 

Thank you Colin, this is exactly what I needed, this point tool path will work better than what I have been doing. 

[Colin Gilchrist]

3 minutes ago, medaq said:

 

Thank you Colin, this is exactly what I needed, this point tool path will work better than what I have been doing. 

Glad that worked for you. I'm always amazed how few people even know about the Point Toolpath. It has been available in the software for decades, but so many people don't need the functionality, so they never get the opportunity to use the path.

After you create the Point Toolpath, you can right-click on the Operation, and choose Toolpath Editor. You can then use the Toolpath Editor to insert a "M00" machine stop, and trigger any function you would like to output using the Canned Text function. You'll have to modify the Canned Text section of the post, so that it will output your custom code, but that is exactly what the Canned Text function is designed to support; custom code, and the ability to output it "anywhere" within your path by making Toolpath Edits. The possibilities with Canned Text are almost limitless...