Editing toolpath?

[Darin]

Hello,

 

I have a simple part that has a moon shaped contour path that I would like to edit the toolpath to a G00 after the lead in and lead out of the path. How do I do this? I have sample code that I edited like I want... But I would like MasterCam to post this way... I have X5..

 

Thanks

 

 

 

N2300 M08

N2310 G00 G17 G90 G55 A0. X-2.4129 Y3.2879 S3200 M03

N2320 G43 H4 Z1. T2

N2330 Z.25

N2380 G01 Z-1.98 F250.

N2390 G41 D4 X-1.5114 Y2.4959 F125.

N2400 G03 X-.4604 Y2.4943 I.5264 J.5991

N2410 G01 G40 X.4434 Y3.2836

N2420 G00 X-2.436 Y3.2616 <----------------------------------- G00

N2430 G01 G41 D4 X-1.5345 Y2.4696 F125. <----------------------- Change Back To G01

N2440 G03 X-.4374 Y2.4679 I.5495 J.6254

N2450 G01 G40 X.4665 Y3.2573

N2460 G00 X-2.4591 Y3.2353

N2470 G01 G41 D4 X-1.5576 Y2.4433 F125.

N2480 G03 X-.4144 Y2.4416 I.5726 J.6517

N2490 G01 G40 X.4895 Y3.2309

N2500 G00 X-2.4822 Y3.209

N2510 G01 G41 D4 X-1.5807 Y2.417 F125.

N2520 G03 X-.3914 Y2.4152 I.5957 J.678

N2530 G01 G40 X.5125 Y3.2045

N2540 G00 X-2.5053 Y3.1827

N2550 G01 G41 D4 X-1.6038 Y2.3907 F125.

N2560 G03 X-.3684 Y2.3889 I.6188 J.7043

N2570 G01 G40 X.5355 Y3.1782

N2580 G00 X-2.5284 Y3.1564

N2590 G01 G41 D4 X-1.6269 Y2.3644 F125.

N2600 G03 X-.3453 Y2.3625 I.6419 J.7306

N2610 G01 G40 X.5585 Y3.1518

N2620 G00 X-2.5515 Y3.1301

N2630 G01 G41 D4 X-1.65 Y2.3381 F125.

N2640 G03 X-.3223 Y2.3361 I.665 J.7569

N2650 G01 G40 X.5816 Y3.1254

N2660 G00 X-2.5746 Y3.1038

N2670 G01 G41 D4 X-1.6731 Y2.3118 F125.

N2680 G03 X-.2993 Y2.3098 I.6881 J.7832

N2690 G01 G40 X.6046 Y3.0991

N2700 G00 X-2.5977 Y3.0775

N2710 G01 G41 D4 X-1.6962 Y2.2855 F125.

N2720 G03 X-.2763 Y2.2834 I.7112 J.8095

N2730 G01 G40 X.6276 Y3.0727

N2740 G00 X-2.6208 Y3.0513

N2750 G01 G41 D4 X-1.7193 Y2.2592 F125.

N2760 G03 X-.2532 Y2.257 I.7343 J.8358

N2770 G01 G40 X.6506 Y3.0464

N2780 G00 X-2.6274 Y3.0437

N2790 G01 G41 D4 X-1.7259 Y2.2517 F60.

N2800 G03 X-.2467 Y2.2495 I.7409 J.8433

N2810 G01 G40 X.6572 Y3.0388

N2820 G00 Z1.

N2830 M09

N2840 M05

N2850 G91 G28 Z0.

N2860 G28 Y0. A0.

N2870 G90

N2880 M30

[Darin]

Hello,

 

I have a simple part that has a moon shaped contour path that I would like to edit the toolpath to a G00 after the lead in and lead out of the path. How do I do this? I have sample code that I edited like I want... But I would like MasterCam to post this way... I have X5..

 

Thanks

 

 

 

N2300 M08

N2310 G00 G17 G90 G55 A0. X-2.4129 Y3.2879 S3200 M03

N2320 G43 H4 Z1. T2

N2330 Z.25

N2380 G01 Z-1.98 F250.

N2390 G41 D4 X-1.5114 Y2.4959 F125.

N2400 G03 X-.4604 Y2.4943 I.5264 J.5991

N2410 G01 G40 X.4434 Y3.2836

N2420 G00 X-2.436 Y3.2616 <----------------------------------- G00

N2430 G01 G41 D4 X-1.5345 Y2.4696 F125. <----------------------- Change Back To G01

N2440 G03 X-.4374 Y2.4679 I.5495 J.6254

N2450 G01 G40 X.4665 Y3.2573

N2460 G00 X-2.4591 Y3.2353

N2470 G01 G41 D4 X-1.5576 Y2.4433 F125.

N2480 G03 X-.4144 Y2.4416 I.5726 J.6517

N2490 G01 G40 X.4895 Y3.2309

N2500 G00 X-2.4822 Y3.209

N2510 G01 G41 D4 X-1.5807 Y2.417 F125.

N2520 G03 X-.3914 Y2.4152 I.5957 J.678

N2530 G01 G40 X.5125 Y3.2045

N2540 G00 X-2.5053 Y3.1827

N2550 G01 G41 D4 X-1.6038 Y2.3907 F125.

N2560 G03 X-.3684 Y2.3889 I.6188 J.7043

N2570 G01 G40 X.5355 Y3.1782

N2580 G00 X-2.5284 Y3.1564

N2590 G01 G41 D4 X-1.6269 Y2.3644 F125.

N2600 G03 X-.3453 Y2.3625 I.6419 J.7306

N2610 G01 G40 X.5585 Y3.1518

N2620 G00 X-2.5515 Y3.1301

N2630 G01 G41 D4 X-1.65 Y2.3381 F125.

N2640 G03 X-.3223 Y2.3361 I.665 J.7569

N2650 G01 G40 X.5816 Y3.1254

N2660 G00 X-2.5746 Y3.1038

N2670 G01 G41 D4 X-1.6731 Y2.3118 F125.

N2680 G03 X-.2993 Y2.3098 I.6881 J.7832

N2690 G01 G40 X.6046 Y3.0991

N2700 G00 X-2.5977 Y3.0775

N2710 G01 G41 D4 X-1.6962 Y2.2855 F125.

N2720 G03 X-.2763 Y2.2834 I.7112 J.8095

N2730 G01 G40 X.6276 Y3.0727

N2740 G00 X-2.6208 Y3.0513

N2750 G01 G41 D4 X-1.7193 Y2.2592 F125.

N2760 G03 X-.2532 Y2.257 I.7343 J.8358

N2770 G01 G40 X.6506 Y3.0464

N2780 G00 X-2.6274 Y3.0437

N2790 G01 G41 D4 X-1.7259 Y2.2517 F60.

N2800 G03 X-.2467 Y2.2495 I.7409 J.8433

N2810 G01 G40 X.6572 Y3.0388

N2820 G00 Z1.

N2830 M09

N2840 M05

N2850 G91 G28 Z0.

N2860 G28 Y0. A0.

N2870 G90

N2880 M30

 

 

From what I can see this is more of a lead in and lead out issue for me... I need to use wear comp and have to use multi passes at full depth.. This causes major issues making a in closed chain and using tool path edit.. If the lead in & out page had a tab that said on the lead out side... rapid to lead in and keep tool down.... This would work... Is this on X6? Seams like it is much easier for me just to edit code.... But if I forget to do this before sending they loose time on runtime... We do thousands of these.. Thanks

[Teh Bear without Brains kinda idiot]

i WOULD USE OTHER TOOLPATH FOR YOUR PART ,Darin .

I mean open pocket

Way more effective .

 

HTH

[Justin Beebe at Folsom Tool]

In your operation manager right click on the toolpath you want to edit then select Toolpath Editor. The Toolpath Editor will give you several options to edit your toolpath at any point. It takes a little while to get used to but can help make your toolpaths more efficient. I would use 2D highspeed Core Mill for that part. Open pocket doesn't rapid between cutting passes. With Core Mill you will have the option to rapid back to the starting position in between cuts or move with a really high feedrate between cuts. Plus you should be able to cut faster in general and not have to worry about burying the tool in the material.

[Guest]

i WOULD USE OTHER TOOLPATH FOR YOUR PART ,Darin .

I mean open pocket

Way more effective .

 

HTH

 

 

Good use for a dynamic contour as well

[Redfire427]

2D HST toolpaths are your friend here. Learn it..........love it.

 

Carmen

[MotorCityMinion]

Another option, although it's old school.

 

1st, reduce those lead in / out values. In this case, I typically use the adjust start of contour function, both entry and exit. You may need an arc to smooth things out or you could use those tangent lines created in the second picture, shortened up, as your chain.

 

Create a line parallel to the side face, offset by half your tool dia. and what you wish to use for a lead in value. I'd use .10 as a lead in for a total of .475. You could go shorter, relative to the amount of stock left on the perimeter.

 

Tool path, trim and it will prompt you to select a region on either side of the line.

 

Now back plot and tweak your lead-in values to suit. Thousands of parts? I'd snug it up quite a bit.

 

Optimally, I'd do what Redfire suggested, 2d HST, as this will back feed at rapid speeds and keep your tool down. Still learn how to use the trim function as it works well with all the tool paths I've tried.

[Darin]

Thanks for th info guys.... I tried open pocket and 2D HST toolpaths... From what I can find none of them let me use multi pass with rough like counter. Also most ask me for two chains why? It should be a simple open chain like is pictured... Simple counter is all most there.. just need added rapid moves and finish feed rate.. I will try again with others 2D HST... I am trying tool path edit some more also... I am limited on program time... We are a full job shop they give you only 1 hour max to program or you can be docked pay.. Time is $ in the new job shop world... Trying to get China work back.... The HST seams to be for pockets.. I need to make full depth cuts 1.970 deep at 650 SFM & 10 .025 .035 radially cuts... The new end mill technology loves this.. This is a 17-4 harden stainless piece and this method beats any indexable so far... I got 300 pieces with one endmill... If someone would like to take my file and show me how easy the 2D HST tool path will work for what I want that would be great.... Thanks

[gcode]

I don't have Mastercam on this machine yet.

 

2d HS dynanic toolpaths need 2 chains

 

One is stock

the other is stock minus cutpath

 

draw a rectangle that represents your stock

 

translate/copy it up .100 and trim your your cut chain out of the second rectangle

 

choose 2d dynamic core and chain both of them.. that should get you started..

 

 

 

Once you get that wired

 

they give you only 1 hour max to program or you can be docked pay..

 

get the he!! out of the sweat shop you're working in

 

docking your pay is NOT legal

[Darin]

Once you get that wired

 

 

 

get the he!! out of the sweat shop you're working in

 

docking your pay is NOT legal

 

 

Thanks for the info I will try that.. I do alot of programming at home and bring to work so I have less time on it.. I know that it is kind of a sweat shop but they give big bonuses if I get it done faster and with less issues... They are the few shops in this area that are booming with work and giving China compitition...Also the pay is really high here (38 a Hr + bonuses) so it is hard to complain..

[Redfire427]

To use the 2D HST toolpath on that curve, you would have to break the arc at the midpoint, so your first rail would be from the top of the arc to the midpoint, and the second rail would be from the bottom of the arc to the midpoint. If my memory serves me correctly, you would also have to shorten the ends of the arc to allow a space between the curves. This would be using the peel mill approach. This toolpath will work extremely well, but will require a follow-up contour operation to remove the "flat section" that is left at the gap between the two rails. Don't give up on this type of strategy. Once you figure out what works best for your application, you will completely forget about the "legacy" toolpaths.

 

Carmen