5-AXIS ROUTER BEGINNER

[Mr. Wizzard]

So, we have a new DMS 5-axis, head-head router for trimming plasitc vac-forms. I have no idea how to even begin. It has a "teach-in" option that allows you to jog the machine around and record/playback the moves. I have done this just so the higher-ups can see it progressing, but it's not efficient at all. I have just been sent the Post for it from In-House. All i did was program a 3-axis contour and the post has so many errors I can't even begin to explain them.

I can't say I did it right, because I don't know. I would like to think I have a pretty decent handle on very complicated programming, but I'm a "5-axis Virgin". I did not change any defaults. I have forwarded the Z2G to my reseller and am waiting to hear back.

I want to ask two questions:

What is the best way to begin learning the basics to 5-axis, in addition to the tutorials?

Does anyone have experience with DMS 5-axis routers programmed with Mastercam or suggestions for me.

Thanks All!

[Colin Gilchrist]

Hi CNC,

 

I've run a DMS with a Fanuc 21i (I think) controller. It was pretty standard compared to other 5 axis gantrys I've run before. The first step you need to take is to read and understand the control manual and programming manual for this machine. The programming manual should specify the layout of the machine's axis system and the way that program zero and tool length compensation is used.

 

The basics for 5 axis Mastercam programming can be learned from a tutorial pretty well. The hard part is figuring out how the machine's gcode is formatted and how to get Mastercam to output the code so the machine will read it.

 

Try this, make a copy of your PST file and then open the copy in the Mastercam X Text editor (make a copy so you don't mess up the original). At the top of the PST file is usually a file header with a bunch of comments about how the post is setup and how to control certain aspects of the gcode output, by using the Misc. Integers and Misc. Real Numbers to control the code output.

 

In addition, most 5 axis posts use some of the tool length parameters to calculate the proper Z values. This all depends on your post of course.

 

I would recommend you contact your reseller or another person to come into your company and do some "hands on" training with you, your post, and Mastercam. Someone can get you up and running in a day or two, versus you spending weeks getting up to speed on your own. Shoot me an email if you need some contacts...

 

Thanks,

[k turk]

once you are sure your post is set up and running properly, colin's suggestion to get 'hand's on' personal training with your machine is a good one. you can't beat a knowledgeable person at your side training you.

 

i found the mastercam handbooks written by charles davis to be very helpful. volume 3 deals specifically with multiaxis machining. you can track it down through the books tab on the forum.

 

k

[KalCam]

Hey cnc,

 

I was handed a new DMS 5-axis router and know exactly what your feeling. Is your machine new? If it is the guy that set it up should have offered training for a day or two.

 

The router here uses a xxxxor control set up using TCP, which makes 5-axis programming/part trimming a snap. One thing to add to Colin's great advice is get that post rock solid working through your reseller. We purchased ours and the post guru helped me out alot. Once your post is right you can focus on programming.

 

I found a old V9 sample file of multi-axis trimming a bed liner. That one file got me up and going on my own and its been one @ell of ride! and this forum is the best.

[Mr. Wizzard]

Thanks for the input guys! I talked briefly to my reseller this morning, but I have a long way to go. I have begun picking through the code on a simple 3-axis contour of a circle. There are so many things wrong when I compare the codes that are output to the Fanuc 8055 programming manual, that I don't even know where to begin.

It seems to me that since I paid 3k for the post and supplied the machine/controller make, serial numbers, etc..... that I should be able to rock and roll.

Even though I don't know much about 5-axis, should I not be able to fly with simple 3-axis programs to get started?

I get return positions that overtravel, metric feedrates of 999999. , and G & M codes that do not exist! Come on......

[KalCam]

Yep! that machine should been running 3-axis at least before that set guy left, even if it was just cutting air. Here's some sample code for my machine.

 

% XXXX XXXXX ,MX

; XXXX XXXXX - 000830

; 25-11-08 09:25

G90

G48 S0 ;TCP OFF

; 3/16 RTR 56-618 TOOL - 2 DIA. OFF. - 2 LEN. - 2 DIA. - .1875

T2

M06

; Pivot Length=0.

G29X

G78

; FRONT NOTCH

D2

G54

G48 S1 ;TCP ON

S18000 M3

M67

G0 G90 X1.3772 Y-.6937 B0. C0.

Z1.

G51 E.004

Z-1.004 B90.

X.9772

G1 X.8772 F100.

Z-.904 F250.

Y-.6928 Z-.8091

Y-.6862 Z-.7431

Y-.6725 Z-.6746

Y-.6531 Z-.6106

Y-.6277 Z-.5489

Y-.5968 Z-.4904

[Mr. Wizzard]

Now, that I can understand! I can actually make sense of that!

Here is what I got for contouring a 20inch square, with the back left corner 50 and 40 inches from origin in X and Y respectively:

00000

;MASTERCAM - X

;MCX FILE - C:CAM PROGRAMSMCAMFILESR&D5-AXISSQUARE CONTOUR.MCX

;MATERIAL - ALUMINUM INCH - 2024

;PROGRAM - NEW TEST.NC

;DATE - DEC-04-2008

;TIME - 1:17 PM

;EXPIRY DATE=DD-MM-YY - 02-02-2009

;POST LICENSE - IN-HOUSE SOLUTIONS

 

;T3 - 1/4 FLAT ENDMILL - D0 - D0 - D0.2500"

N100 G00 G17 G70 G80 G90

N110 G40 G44

N120 G49

N130 G48 S0 ;TCP OFF

N140 M11 ; UNSLAVE U AND X TABLES

N150 G00 G53 Z0.

N160 X13. Y96.

N170 B0. C0.

N180 (ORGX56 = 67.4722)

N190 (ORGY56 = 4.1245)

N200 (ORGZ56 =-35.512)

N210 (ORGU56 =-67.4722)

N220 (ORGB56 = 0.0)

N230 (ORGC56 = 0.0)

N240 G56

N250 (ORGX54 = 0.0)

N260 (ORGY54 = 0.0)

N270 (ORGZ54 = 0.0)

N280 (ORGU54 = 0.0)

N290 (ORGB54 = 0.0)

N300 (ORGC54 = 0.0)

N310 G05

N320 G80

N330 G40

N340 G48 S0

N350 M66 ; TOOL AIR OFF

N360 ;TOOLPLANE NAME - TOP

N370 T3 ; 1/4 FLAT ENDMILL

N380 M06

N390 ;MAX - Z.25

N400 ;MIN - Z-1.

N410 S15000

N420 M03

N430 G04 K200

N440 G49 X0Y0Z0A0B0C90.

N450 G54

;M65 ; TOOL AIR ON

N460 M63 ; TABLE X VACUUM ON

N470 D3

N480 G05

N490 G00 G17 G90 X50. Y-40.

N500 B0. C0.

N510 G43 D3 Z.25

N520 G04 K400

N530 Z.1

N540 G94 G01 Z-1. F999999.

N550 X70.

N560 Y-60.

N570 X50.

N580 Y-40.

N590 G00 Z.25

N600 G70 G80 G90

N610 G40 G44

N620 G48 S0 ;TCP OFF

N630 G49

N640 G53

N650 G00 Z0.

N660 M05

N670 G01 X13. Y96. F1000.

N680 M11 ;UNSLAVE U AND X TABLES

N690 ;M64; TABLE X VACUUM OFF

N700 ;M62; TABLE U VACUUM OFF

N710 M30

 

 

Does this look normal?

[KalCam]

Wow! that looks like a mess. This is what I get for just simple path around a 20 x 20.

 

% 20X20 TEST ,MX

; 20X20 TEST - 000500

; 04-12-08 11:42

G90

G48 S0 ;TCP OFF

; 1/4 RTR 56-625 TOOL - 3 DIA. OFF. - 3 LEN. - 3 DIA. - .25

T3

M06

; Pivot Length=0.

G29X

G78

D3

G54

G48 S1 ;TCP ON

S17000 M3

M67 ;AIR NOZZLE ON

G0 G90 X-.125 Y0. B0. C0.

Z1.

G51 E.002

Z.75

G1 Z0. F100.

Y20. F300.

G2 X0. Y20.125 I.125 J0.

G1 X20.

G2 X20.125 Y20. I0. J-.125

G1 Y0.

G2 X20. Y-.125 I-.125 J0.

G1 X0.

G2 X-.125 Y0. I0. J.125

G1 Z.5

G0 Z1.

M5

M68 ;AIR NOZZLE OFF

M62 ;VACUUM OFF

G48 S0 ;TCP OFF

G53

M30

 

This machine has only one table.

[wildcat99]

Just start a new thread "Wanted, Free Post" and you'll get lots of help! j/k

 

quote:

---

I have just been sent the Post for it from In-House.

---

Keep after them they will make it right. Maybe they sent the wrong post??

[Mr. Wizzard]

HA HA, I've seen the responses for "Wanted:Free Post"

I've sent my files and I'm playing phone tag right now.