FeatureCAM post for Brother C00 control?

Anybody? Since support is absolutely a worthless piss-poor joke now.......
I am going to start out editing code from my HAAS post for now I guess.
But, I am not a big fan of hand editing code. Esp. the very looong programs I am going to be posting.
And, I am not good enough in X-build to make my own post.

Wheelie,

This for your new Brother pallet machine? You're just doing prismatic (2.5D) work, right? Reason I ask, we have post for our R650 which I'm glad to send over, but we have 4th on both pallets and create setups at each location. I'm little concerned about how it will work if used with multiple fixture offsets, etc. I just don't want to send anything that causes more problems than it solves. PM me. I'm in and out of here over next few days, so bear with me

Fred

Message sent!

Your haas post should work fine. Literally the only thing you will need to change is the tapping cycle.
G77 instead of G84

G77G98Z-.250R.050S1000J20. (1/4-20 thread)
G77G98Z-.250R.050S1000I.7 (m4x.7 thread)

Get it up and running and you can implement the G100 Tool change call later to save a few seconds but honestly I hardly ever use it. The machines move fast enough as it is.

dstryr said:

Your haas post should work fine. Literally the only thing you will need to change is the tapping cycle.
G77 instead of G84

G77G98Z-.250R.050S1000J20. (1/4-20 thread)
G77G98Z-.250R.050S1000I.7 (m4x.7 thread)

Get it up and running and you can implement the G100 Tool change call later to save a few seconds but honestly I hardly ever use it. The machines move fast enough as it is.

Click to expand...

Thanks Dennis! No tapping needed (yet)!

And you need to change the tool change cycle!

The use of G100 is a great feature,

( T )
( DATE - 06-03-18 )
( TIME - 16:31 )

(T31-NO. 75 DRILL-H31)

G0G17G40G49G80G90

(NO. 75 DRILL)
G0G90G54G100T31X0.Y0.A0.S12733M3
G43H31Z.1
G99G81Z0.R.1F4.07
X-1.5262Y.6607
G80
M5
G91G28Z0.M19
M30

solidworkscadman said:

And you need to change the tool change cycle!

The use of G100 is a great feature,

( T )
( DATE - 06-03-18 )
( TIME - 16:31 )

(T31-NO. 75 DRILL-H31)

G0G17G40G49G80G90

(NO. 75 DRILL)
G0G90G54G100T31X0.Y0.A0.S12733M3
G43H31Z.1
G99G81Z0.R.1F4.07
X-1.5262Y.6607
G80
M5
G91G28Z0.M19
M30

Click to expand...

That could be done at a later time... It will save 2 seconds vs him getting the first chips made lol

I will look in to G100. But, M6 will work just fine for now. (I think)

Edit: Looks like G100 is how you git er' to do TC and vector in to position at the same time?

wheelieking71 said:

I will look in to G100. But, M6 will work just fine for now. (I think)

Edit: Looks like G100 is how you git er' to do TC and vector in to position at the same time?

Click to expand...

Yes, that is how it's done.
I use a Haas post for other software (bobcad) and works fine except for tapping. Just be sure there isn't a G20 in there, it doesn't like or need that. Some posts were also throwing a G49 n there, not needed or wanted.

I have stumbled on all kinds of little issues trying to get this Brother to run on my HAAS post.
What a pain in the arse, LOL.
I would make a list, but, my head is jello right now.
I got it to do a simple operation. But, it took a bunch of editing.
I would have to go compare the code I posted to what actually ran to make the list.
Maybe later, got to run wifey to airport right now..............

Well, countless hours later (in XBUILD) and I finally have a post that will run with zero hand editing.
Thanks for nothing AutoDICKS. You guys suck ass.

My ballon-knot will still be tight as hell proving programs I am sure, because, well I wrote the damn post. And, I really have no business doing that.
But, I am at least moving forward.

Here is a non edited program as-posted:

(PIGNOSE ST-104 ALL MILL)
( T1 = LITTLE DADDY )
( T2 = #23 DRILL )
( T3 = .1562 3FL CARB EM )
( T4 = .250 2FL 90' )
N1 G00 G91 M05 G80
T1 M6 ( LITTLE DADDY 1.25 DIA. )
G90 G54 X1.8125 Y1.2547 S10000 M3
G43 H1 Z1.1
/M8
Z0.2
G1 G17 Z0.02 F75.0
Y-1.1947
G0 Z1.1
X1.0625 Y1.3993
Z0.2
G1 Z0.02
Y-1.3393
G0 Z1.1
X1.8125 Y1.2547
Z0.12
G1 Z0. F50.0
Y-1.1947
G0 Z1.1
X1.0625 Y1.3993
Z0.12
G1 Z0.
Y-1.3393
G0 Z1.1
M9
G00 G91 G28 Z0 M05
M1

( HOLE1 )
N2 G00 G91 M05
T2 M6 ( #23 DRILL 0.154 DIA. )
G90 G54 X0.875 Y-0.2275 S6000 M3
G43 H2 Z1.1
/M8
G81 G98 Z-0.2463 R0.1 F18.0
G0 G80 Z1.1
X1.5
G81 G98 Z-0.2463 R0.1 F18.0
G0 G80 Z1.1
Y0.2875
G81 G98 Z-0.2463 R0.1 F18.0
G0 G80 Z1.1
X0.875
G81 G98 Z-0.2463 R0.1 F18.0
G0 G80 Z1.1
M9
G00 G91 G28 Z0 M05
M1

( ROUGH1 POCKET3 )
N3 G00 G91 M05
T3 M6 ( .1562 3FL CARB EM 0.1562 DIA. )
G90 G54 X1.5139 Y-0.0713 S10000 M3
G43 H3 Z1.1
/M8
Z0.1
G1 Z0.01 F35.0
Y-0.2275 Z-0.0033
Y-0.0713 Z-0.0167
Y-0.2275 Z-0.03
Y-0.0713 Z-0.0433
Y-0.2275 Z-0.0567
Y-0.0713 Z-0.07
Y-0.2275 Z-0.0833
Y-0.0713 Z-0.0967
Y-0.2275 Z-0.11
Y0.2875
G3 X1.4861 Y0.2875 I-0.0139 J0.
G1 Y-0.2275
G3 X1.5139 Y-0.2275 I0.0139 J0.
G1 Y-0.0713
Y-0.2275 Z-0.1133
Y-0.0713 Z-0.1267
Y-0.2275 Z-0.14
Y-0.0713 Z-0.1533
Y-0.2275 Z-0.1667
Y-0.0713 Z-0.18
Y-0.2275 Z-0.1933
Y-0.0713 Z-0.2067
Y-0.2275 Z-0.22
Y0.2875
G3 X1.4861 Y0.2875 I-0.0139 J0.
G1 Y-0.2275
G3 X1.5139 Y-0.2275 I0.0139 J0.
G0 Z1.1
X0.8889 Y-0.0713
Z0.1
G1 Z0.01
Y-0.2275 Z-0.0033
Y-0.0713 Z-0.0167
Y-0.2275 Z-0.03
Y-0.0713 Z-0.0433
Y-0.2275 Z-0.0567
Y-0.0713 Z-0.07
Y-0.2275 Z-0.0833
Y-0.0713 Z-0.0967
Y-0.2275 Z-0.11
Y0.2875
G3 X0.8611 Y0.2875 I-0.0139 J0.
G1 Y-0.2275
G3 X0.8889 Y-0.2275 I0.0139 J0.
G1 Y-0.0713
Y-0.2275 Z-0.1133
Y-0.0713 Z-0.1267
Y-0.2275 Z-0.14
Y-0.0713 Z-0.1533
Y-0.2275 Z-0.1667
Y-0.0713 Z-0.18
Y-0.2275 Z-0.1933
Y-0.0713 Z-0.2067
Y-0.2275 Z-0.22
Y0.2875
G3 X0.8611 Y0.2875 I-0.0139 J0.
G1 Y-0.2275
G3 X0.8889 Y-0.2275 I0.0139 J0.
G1 G41 D03 X0.8934 Y-0.217
G3 X0.8949 Y-0.2056 I-0.0414 J0.0114
G1 Y0.2875
G3 X0.8551 Y0.2875 I-0.0199 J0.
G1 Y-0.2275
G3 X0.8949 Y-0.2275 I0.0199 J0.
G1 Y-0.1056
G3 X0.8934 Y-0.0943 I-0.043 J0.
G1 G40 X0.8889 Y-0.0837
G0 Z1.1
X1.4861
Z0.1
G1 Z-0.22
G41 D03 X1.4816 Y-0.0943
G3 X1.4801 Y-0.1056 I0.0414 J-0.0114
G1 Y-0.2275
G3 X1.5199 Y-0.2275 I0.0199 J0.
G1 Y0.2875
G3 X1.4801 Y0.2875 I-0.0199 J0.
G1 Y-0.2056
G3 X1.4816 Y-0.217 I0.043 J0.
G1 G40 X1.4861 Y-0.2275
G0 Z1.1
M9
G00 G91 G28 Z0 M05
M1

( CHAMFER POCKET3 )
N4 G00 G91 M05
T4 M6 ( .250 2FL 90' 0.25 DIA. )
G90 G54 X1.468 Y-0.2275 S10000 M3
G43 H4 Z1.1
/M8
Z0.1
G1 Z-0.06 F60.0
G41 D04 X1.477 Y-0.2555
G3 X1.5047 Y-0.2652 I0.0236 J0.023
X1.538 Y-0.2275 I-0.0047 J0.0377
G1 Y0.2875
G3 X1.462 Y0.2875 I-0.038 J0.
G1 Y-0.2275
G3 X1.5346 Y-0.2432 I0.038 J0.
X1.5335 Y-0.2138 I-0.0301 J0.0136
G1 G40 X1.5094 Y-0.1969
G0 Z1.1
X0.907
Z0.1
G1 Z-0.06
G41 D04 X0.9115 Y-0.1879
G3 X0.913 Y-0.178 I-0.0315 J0.0099
G1 Y0.2875
G3 X0.837 Y0.2875 I-0.038 J0.
G1 Y-0.2275
G3 X0.913 Y-0.2275 I0.038 J0.
G1 Y-0.078
G3 X0.9115 Y-0.068 I-0.033 J0.
G1 G40 X0.907 Y-0.059
G0 Z1.1
X0.4175 Y0.03
Z0.1
G1 Z-0.07
G41 D04 X0.4355 Y0.0411
G3 X0.4431 Y0.0608 I-0.0254 J0.0211
G2 X0.4431 Y0.0608 I0.7444 J-0.0308
X0.4555 Y0.1688 I0.7444 J-0.0308
G3 X0.4526 Y0.1897 I-0.0324 J0.0061
G1 G40 X0.4376 Y0.2046
G0 Z1.1

M9
G00 G91 G28 Z0 M05
G28 Y0
M30

I can not get G100 to work. I am sure it is because I don't know WTF I am doing in XBUILD.
Dumb things to note:
Coolant-on absolutely has to be on its own line.
Can not have a G28 Z0 in the safety line.
It pitched a fit until I figured out how to eliminate the HAAS tool pre-call.
In one of my edits I somehow lost the G28 Z0 on the line before the M1, and it took me forever to figure out how to get it back.
I never did actually. I started over. And managed not to loose it the second time.
And a couple other things I don't remember.
But, that program runs.

You know you definitely need to tell us what tool Little Daddy is now, yes?

If someone would explain G100 I would like to know how it works. I have an A00 control and the manuals are in broken english and I can't quite grasp it.

Check with BrotherFrank to see if that version supports it.
Typical code:
G100 T6 G54 X1.5 Y.5 S7500 M3

Positions and changes tool during the positioning, and of course turns on the spindle.
If you have a pallet/quick turn table machine, it does all this while the table is rotating.
Quite convenient. Minimal wasted time.
I have a bunch of partsI make often with about a 3 minute cycle time. Loading time can take 30 seconds to a minute, depending..... but since the loading is while the machine is cutting on the other side of the table, loading time net is the 3 seconds it takes to rotate. Combine that with the spindle accel/decel of the Brother spinde, and the positioning speed, parts get done efficiently.

Even if I set up and load 4 parts, I still get only the 3 second net load time.

eaglemike said:

Check with BrotherFrank to see if that version supports it.
Typical code:
G100 T6 G54 X1.5 Y.5 S7500 M3

Positions and changes tool during the positioning, and of course turns on the spindle.
If you have a pallet/quick turn table machine, it does all this while the table is rotating.
Quite convenient. Minimal wasted time.
I have a bunch of partsI make often with about a 3 minute cycle time. Loading time can take 30 seconds to a minute, depending..... but since the loading is while the machine is cutting on the other side of the table, loading time net is the 3 seconds it takes to rotate. Combine that with the spindle accel/decel of the Brother spinde, and the positioning speed, parts get done efficiently.

Even if I set up and load 4 parts, I still get only the 3 second net load time.

Click to expand...

What Mike said! I would add a little to the code:

G100 T1 G0 G90 G54 X_ Y_ A_ (and or B if available) S_ M3;
G43 H1 Z.1 M8;
;
;

Some guys put the Z move on the G100 line. I usually don't. You could if you're trying to eek out every last bit of time. Another time saver is don't G91 G28 Z0 at the end of a tool. Just go straight to the G100. I usually leave home moves in until I prove the program out and then take them out. Yes the A00 machines can run G100, so can any G-code Brother back to the early 90s.

gkoenig said:

You know you definitely need to tell us what tool Little Daddy is now, yes?

Click to expand...

I could tell you, but then he would kill us both!

BROTHERFRANK said:

What Mike said! I would add a little to the code:

G100 T1 G0 G90 G54 X_ Y_ A_ (and or B if available) S_ M3;
G43 H1 Z.1 M8;
;
;

Some guys put the Z move on the G100 line. I usually don't. You could if you're trying to eek out every last bit of time. Another time saver is don't G91 G28 Z0 at the end of a tool. Just go straight to the G100. I usually leave home moves in until I prove the program out and then take them out. Yes the A00 machines can run G100, so can any G-code Brother back to the early 90s.

Click to expand...

BROTHERFRANK, I am really struggling to understand why my machine locks up if the M8 is on any line other than all by itself on its own line.
I can put a block-skip before it. But, it has to be on its own line.

What you typed up there ^^^^^^ "G43 H1 Z.1 M8;" absolutely will not fly in my machine. I have tried countless times.



If I delete it out of that line, it runs fine.
Only thing the manual says for Alarm SM4006 is: Invalid data, the specified format is not correct

wheelieking71 said:

BROTHERFRANK, I am really struggling to understand why my machine locks up if the M8 is on any line other than all by itself on its own line.
I can put a block-skip before it. But, it has to be on its own line.

What you typed up there ^^^^^^ "G43 H1 Z.1 M8;" absolutely will not fly in my machine. I have tried countless times.

View attachment 222821

If I delete it out of that line, it runs fine.
Only thing the manual says for Alarm SM4006 is: Invalid data, the specified format is not correct

Click to expand...

Something weird. They'll help you get it sorted. Works for me.

wheelieking71 said:

BROTHERFRANK, I am really struggling to understand why my machine locks up if the M8 is on any line other than all by itself on its own line.
I can put a block-skip before it. But, it has to be on its own line.

What you typed up there ^^^^^^ "G43 H1 Z.1 M8;" absolutely will not fly in my machine. I have tried countless times.

View attachment 222821

If I delete it out of that line, it runs fine.
Only thing the manual says for Alarm SM4006 is: Invalid data, the specified format is not correct

Click to expand...

Well ... your screenshot shows "/M8" which is invalid. Just saying ...