Need Help with 4th/5th axis cut.

[Jon @ NOWHERE]

I have a part that I am working on. It has a chamfer that starts on the side and curves around to the top. Its kinda hard to explain so I will post a pic in a minute. I am running this part on a Makino A51 and need to program it so that the b-axis moves while the chamfer cutter is cutting. Im having a hard time wrapping my head around this as I have never done a 4th axis cut. Any help is greatly appreciated.

 

Edit: I am using MasterCam X2

 

Jon

[Jon @ NOWHERE]

 

Here is a pic of the part on the tombstone how I will hold it.

[cobra95kev]

I also program similar parts on a Makino A-51.

Unfortunately I have no experience in doing what you need to do. But I am looking forward to hearing the responses you get.

 

If it was me and I needed to get the parts out you could rotate to B315. and just scrub it on there.

 

Good Luck ,

[Guest CNC Apps Guy 1]

If I HAD to do it the way you're proposing, I'd use Curve 5 Axis as I can dictate angle of attack by lines and I can constrain the toolpath to 4 Axis.

[Guest CNC Apps Guy 1]

Look on the FTP in the ftp://www.ppcadcam.com/Mastercam_forum/MCX2_Files/ folder for a Curve 5-Axis Test file.

 

HTH

[Jon @ NOWHERE]

quote:

---

Look on the FTP in the

ftp://www.ppcadcam.com/Mastercam_forum/MCX2_Files/

folder for a Curve 5-Axis Test file.

 

HTH

---

I tried what was shown in that file and it seemed to work, but i cant verify it without some code. I guess I will have to wait til I finish and then run it through vericut to verify the whole program. Thanks for your help!

 

Jon

[Guest CNC Apps Guy 1]

You're welcome.

[Jon @ NOWHERE]

CNC Apps Guy, why is it that the 5 axis curve works that way? I've just about beat my head against the wall trying to get that to work, you put me on to that test file, I follow that example and apply it to my part and it appeared to give me the results I was needing. I just don't understand all the options. Is there anything that might explain it all, that I could possibly get my hands on?

 

Edit: I guess I should mention that I am somewhat self-taught with Mastercam.

 

Again thanks for your help!

Jon

[Guest CNC Apps Guy 1]

The bottom curve is what drives the tool - what it follows along. The lines that are perpendicular to the curve are what tells the toolpath what vector to follow. On the arc, the two lines basically tell it to fan between the two lines. I selected the lines from the part closest to the chain. Hopefully that makes sense.

[Jon @ NOWHERE]

Yeah that makes a little sense to me. The curve that drives the tool, does the center of the tool follow that path? Meaning that I need to create the lines for the tool to follow offset from the part in order to get the desired results?

 

 

Jon

[Jon @ NOWHERE]

Something is not right. Here is the code for just one of the cuts:

 

N1 G00 G17 G20 G40 G80 G90 G94

N2 (CUT CHAMFER ON CLEVIS)

N3 M11

N4 T154 M06 (35.5 DEGREE CHAMFER MILL)

N5 T154

N6 G00 G90 G54.1 P11 G17 X8.937 Y7.3572 B270. S4074 M303

N7 G43 Z9.0637 H1 D2 M302

N8 M08

N9 Z10.3773

N10 G94 G01 Z5.0637 F6.

N11 X9.037 Z5.0638 F81.48

N12 X9.137 Z5.0639

N13 X9.237 Z5.064

N14 X9.337

N15 X9.4369 Z5.0641

N16 X9.537 Z5.0642

N17 X9.637 Z5.0643

N18 X9.737 Z5.0644

N19 X9.837 Z5.0645

N20 X9.937

N21 X10.0284 Z5.0646

N22 G93 G91 X.6204 Z-1.3675 B-352.47 F1000.

N23 G90 X11.1531 Z1.8516 B287.098 F1000.

N24 X11.3272 Z-.3349 B298.049 F1000.

N25 X10.9768 Z-2.8991 B310.953 F1000.

N26 X9.9905 Z-5.4231 B324.438 F1000.

N27 X8.6358 Z-7.4019 B336.333 F1000.

N28 X7.0804 Z-8.9002 B347.005 F1000.

N29 X5.6702 Z-9.8494 B355.369 F1000.

N30 X4.8283 Z-10.2782 B0. F1000.

N31 G94 F81.48

N32 X4.7912 Z-10.2803

N33 G00 Z-15.5939

N34 Z-14.2803

N35 G91 G28 Z0.

N36 M06

N37 M30

 

I'm not sure if it has something to do with my post processor or if it is the way I have it set up. The wcs is set to the center of the tombstone on the bottom. And I change the gview to what I need it at and the t/c plane to equal the gview. What am I doing wrong?

 

Please Help

Jon

[Guest CNC Apps Guy 1]

Don't ghange the G-View. You want your WCS to be top and your T/C planes to be Front. This should force your B's and Z's to be what they should be.

 

Hopefully your machine supports inverse time.

[Jon @ NOWHERE]

I have tried that and it doesnt seem to work. Or I am not doing exactly what you are saying. But to me by looking at code it appears that the x and z are not following the b. So when it rotates while trying to cut and then continues cutting it is still as if it didnt rotate at all. Hence my z going into the negatives. Here they want us to program with our y coming from the bottom of the pallet and our x and z coming from the center of the pallet. So our z's are always positive unless we are programming in incremental mode.

[Jon @ NOWHERE]

If there is a way for it change offsets dynamically while in the middle of the cut I think that is the route it needs to take. This problem is the one thing that is holding me up from completing this program. We have a guy coming from our reseller to work on some of our posts this Thursday, but I would like to get this problem hammered out or at least know if it is something I am doing or the post is doing before he gets here.

[Guest CNC Apps Guy 1]

If you can put this on the FTP, I'd be happy to take a look...

[Jon @ NOWHERE]

The file is Here.

 

Thank you for taking the time to help me.

 

After looking at it, if you got any tips or pointers for me, I'm eager to learn.

 

Edit: The two 5 axis cuts are at the bottom, I have been playing with both trying to get it to output the code the way I want it. So one is set to front for t/c plane, the other is set to left.

 

Jon

 

[ 01-27-2008, 08:13 PM: Message edited by: FAS_MaKiNoMaN ]

[Guest CNC Apps Guy 1]

Linky

 

Just adjust entry exit as necessary...

[Jon @ NOWHERE]

When I post it I still get negative z's, that will cause a crash. Not sure if you have a different post than I do either. Because at one point it gave me the following error:

 

ERROR - POST ROTARY AXIS ASSIGNMENT ('rot_on_x') IS DISABLED

 

It needs to use both the left and front offsets. If you dont mind could you post it and post the code here for one of the cuts, that way if it is different from you then I will know that something is up with my post file.

[Guest CNC Apps Guy 1]

code:

---

%

O0000(8INTOMBSTONEOP1AND2_CNCAG-OP01)

(DATE=DD-MM-YY - 27-01-08 TIME=HH:MM - 19:18)

(MCX FILE - C:DOCUMENTS AND SETTINGSCNC-APPS_GUYDESKTOP8INTOMBSTONEOP1AND2_CNCAG.MCX)

(NC FILE - C:DOCUMENTS AND SETTINGSCNC-APPS_GUYDESKTOP8INTOMBSTONEOP1AND2_CNCAG-OP01.NC)

(MATERIAL - ALUMINUM INCH - 7075)

( T154 | 35.5 DEGREE CHAMFER MILL | H0 | D0 | WEAR COMP | TOOL DIA. - .375 )

N100 G20

N102 G0 G17 G40 G49 G80 G90

N110 T154 M6

N112 G0 G90 G54 X8.937 Y7.3572 B90. S4074 M3

N114 G43 H0 Z9.0637

N116 M8

N118 Z5.1637

N120 G1 Z5.0637 F40.74

N122 X9.0374 Z5.0631 B90.004 F3.49

N124 X9.1377 Z5.0625 B90.009

N126 X9.2381 Z5.0619 B90.013

N128 X9.3385 Z5.0612 B90.017

N130 X9.4388 Z5.0606 B90.021

N132 X9.5393 Z5.0599 B90.026

N134 X9.6397 Z5.0592 B90.03

N136 X9.74 Z5.0585 B90.034

N138 X9.8404 Z5.0578 B90.039

N140 X9.9408 Z5.0571 B90.043

N142 X9.922 Z5.2861 B88.728 F412.47

N144 X9.1552 Z6.588 B80.911 F362.3

N146 X8.0299 Z7.9648 B71.733 F341.69

N148 X6.4464 Z9.3241 B60.987 F321.58

N150 X4.3344 Z10.496 B48.567 F304.98

N152 X2.0774 Z11.177 B36.452

N154 X-.0956 Z11.3737 B25.23 F293.24

N156 X-2.0595 Z11.1845 B15.054

N158 X-3.564 Z10.7904 B6.999

N160 X-4.2599 Z10.5265 B3.13 F306.32

N162 G0 Z10.6265

N164 Z14.5265

N166 Y7.6097

N168 Z10.6265

N170 G1 Z10.5265 F40.74

N172 X-2.9 Z10.9927 B10.597 F299.77

N174 X-1.1212 Z11.3189 B19.943

N176 X.9248 Z11.3346 B30.478

N178 X3.2692 Z10.8822 B42.753

N180 X5.5521 Z9.8941 B55.54 F313.23

N182 X7.3496 Z8.6132 B66.896 F331.61

N184 X8.7308 Z7.1626 B77.224 F353.14

N186 X9.6226 Z5.8461 B85.442 F372.5

N188 X10.0161 Z5.0565 B90.046 F386.24

N190 X9.9158 Z5.0573 B90.042 F3.35

N192 X9.8153 Z5.058 B90.038

N194 X9.7149 Z5.0587 B90.033

N196 X9.6145 Z5.0594 B90.029

N198 X9.5142 Z5.0601 B90.025

N200 X9.4138 Z5.0608 B90.02

N202 X9.3134 Z5.0614 B90.016

N204 X9.213 Z5.062 B90.012

N206 X9.1126 Z5.0627 B90.008

N208 X9.0122 Z5.0633 B90.003

N210 X8.937 Z5.0637 B90.

N212 G0 Z5.1637

N214 Z9.0637

N216 M9

N218 M5

N220 G91 G28 Z0.

N222 G28 X0. Y0. B0.

N224 M30

%

---

This was posted using an unalterred generic HMC MC/CD that comes with Mastercam.

 

HTH

[Jon @ NOWHERE]

Now that looks more like the code that should mine should be putting out, with the exception that the it the b90-0 should be b0-b270 and the x's should have their positive and negative signs reversed. I will call our reseller tomorrow, and maybe they can tell me why my post will not output the correct numbers. I finally found our info to verify in mastercam and what I put in for my paths yielded similar results as yours, in the verify part that is. Thanks for all your help, its time for me to go I've been here working on this program for 15 hours already!!

 

Jon

[Guest CNC Apps Guy 1]

You're Welcome Jon. Glad to be of help.

 

BTW; Welcome to the Forum!

[Jon @ NOWHERE]

Thank You, I either dont have that generic post that you used or I dont know how to find it on the cd. I just installed X2 MR2, and it only installed 2 machine definitions. So I aint sure what I am doing wrong. I guess I will have to address that with the resellers to cause I must've not followed directions when installing it lol.

 

Edit: Ok I figured out how to install the extra machine definitions off the disk. And I found the post that would give me the same code that you have posted. So at least I am somewhat closer than before.

 

[ 01-28-2008, 07:39 AM: Message edited by: FAS_MaKiNoMaN ]