feed rate and rapid one tool path?

[RDEnright]

I could desperately use some help with a question that neither my customer service nor mastercam help line, could help me with. I would greatly appreciate any help and/or suggestions with this.

Question - I am trying to bore a hinge with a feed rate, rapid through an open section, and then a feed rate to cut a second bore. I tried everything I can think of. Even with two tool paths setup,

after the first bore - I cant get it to stay where it is for the second path to pick it up, before it retracts or clears back to top of part after first cut. I have tried messing around alittle bit with

points, but I think its just a matter of clearance/retract/top of stock - setup in a certain way, that I just cant figure out.

[Dtm]

I could desperately use some help with a question that neither my customer service nor mastercam help line, could help me with. I would greatly appreciate any help and/or suggestions with this.

Question - I am trying to bore a hinge with a feed rate, rapid through an open section, and then a feed rate to cut a second bore. I tried everything I can think of. Even with two tool paths setup,

after the first bore - I cant get it to stay where it is for the second path to pick it up, before it retracts or clears back to top of part after first cut. I have tried messing around alittle bit with

points, but I think its just a matter of clearance/retract/top of stock - setup in a certain way, that I just cant figure out.

 

Not sure if there is a way for this. Why don't you just manually change the program? G1 z-.500 F5. , G1 Z-1. F100. , G1 Z-1.500 F5. Something like this.

[EX-wccprogrammer]

Custom Drill Cycle.

 

Can do exactly what you want it to do.

 

I wrote one very similar to this.

[EX-wccprogrammer]

Or you could treat it as a 3-D Contour for each section of bore with no retract between. If you use a regular drill cycle, it will automatically retract between holes.

[Dtm]

Custom Drill Cycle.

 

Can do exactly what you want it to do.

 

I wrote one very similar to this.

 

I have never used the custom drill cycle. Could you show some screen shots?

[Guest]

This was a simple solution but I used the Toolpath editor

 

Right click on the toolpath, tool path editor, find the offending points and delete the retract points, leaving only the rapid down point

 

N100 G20

N102 G0 G17 G40 G49 G80 G90

N104 T239 M6

N106 G0 G90 G54 X0. Y0. S1069 M3

N108 G43 H239 Z2.

N110 Z.1

N112 G1 Z-.5 F15.

N114 Y.125 F25.

N116 X.0324 Y.2457

N118 G3 X0. Y.25 R.125

N120 Y-.25 R.25

N122 Y.25 R.25

N124 X-.0324 Y.2457 R.125

N126 G1 X0. Y.125

N128 Y0.

N130 G0 Z-1.4

N132 G1 Z-2. F15.

N134 Y.125 F25.

N136 X.0324 Y.2457

N138 G3 X0. Y.25 R.125

N140 Y-.25 R.25

N142 Y.25 R.25

N144 X-.0324 Y.2457 R.125

N146 G1 X0. Y.125

N148 Y0.

N150 G0 Z-1.25

N152 Z2.

N154 M5

N156 G91 G28 Z0.

N158 G28 X0. Y0.

N160 M30

[jesse@desemco]

Use point toolpaths.

G0 (point) over part

G1 (point) thru 1st bore

G0 (point) over 2nd bore

G1 (point) thru 2nd bore

G0 (point) back out

 

All in 1 toolpath

[EX-wccprogrammer]

There are none supplied with MasterCam, you have to have them written in your post. After you write and name them, just hang names in the corresponding cycle in the control definition. Then when you pull down your drilling menu, it looks kind of like this: (see attached)

CustomMenu.pdf

[john316]

Use point toolpaths.

G0 (point) over part

G1 (point) thru 1st bore

G0 (point) over 2nd bore

G1 (point) thru 2nd bore

G0 (point) back out

 

All in 1 toolpath

 

 

^^^^^^

[RDEnright]

Wow, I cant believe the quick time and quality of these reply's. Better than my tech help! Thanks so much for the help everyone!! Here is another one that no one can help me with -- Anyone know where I can find some good, detailed information on how to setup a custom machine for the mastercam simulation? I can build the parts no problem in SW, but am having a hell of a time trying to get everything setup in mcx. The help that comes with mastercam just isnt enough to help me grasp what to do.

[RDEnright]

This was a simple solution but I used the Toolpath editor

 

Right click on the toolpath, tool path editor, find the offending points and delete the retract points, leaving only the rapid down point

 

I tried this, but I used a bore cycle for the boring bar, and when I goto that, its just a "point" and cant really alter anything

[RDEnright]

^^^^^^

 

yes! that worked nicely. thank you!