[dougputt]

Hi

When using x5 what can I change in the linking parameters or post to stop the cutter length from canceling above part and driving the tool into the part? This only happens when I use tools that have + length compensation.

DP

[Bm150]

Post some code so we can see what's happening...

Sent from my HTC One using Tapatalk

[dougputt]

15 G20
N16 G0 G17 G40 G80 G90
N17 ( 1/8 SPOTDRILL TOOL - 4 DIA. OFF. - 4 LEN. - 4 DIA - .125 )
N18 ( DOUGS VMC 40 )
N19 ( CENTER )
N20 T4 M6
N21 A-0.
N22 G0 G90 S2139 M3 E11 X.5 Y4.5
N23 H4 Z2. M8
N24 G81 G98 X.5 Y4.5 Z-.1425 R0.1 F3.
N25 X3.5
N26 X.5 Y.5
N27 G80
N28 M5 M9
N29 G90 H0 Z0.
N30 M1
N31 ( .167 PILOT DRILL (21?) TOOL - 7 DIA. OFF. - 7 LEN. - 7 DIA - .167 )
N32 ( DOUGS VMC 40 )
N33 ( PILOT HOLE )
N34 T7 M6
N35 G0 G90 S1900 M3 E11 X.5 Y4.5
N36 H7 Z2. M8
N37 G83 G98 X.5 Y4.5 Z-.5602 R0.1 Q.0501 F2.74
N38 X3.5
N39 X.5 Y.5
N40 G80
N41 M5 M9
N42 G90 H0 Z0.
N43 M1
N44 ( .381 TIN DRILL BIT TOOL - 5 DIA. OFF. - 5 LEN. - 5 DIA - .381 )
N45 ( DOUGS VMC 40 )
N46 ( THROUGH HOLE )
N47 T5 M6
N48 G0 G90 S2406 M3 E11 X.5 Y4.5
N49 H5 Z2. M8
N50 G83 G98 X.5 Y4.5 Z-.7245 R0.1 Q.1143 F3.5
N51 X3.5
N52 X.5 Y.5
N53 G80
N54 M5 M9
N55 G90 H0 Z0.
N56 E0 X0 Y0
N57 M30
%
%

[Bm150]

Guess it's the h0 z0, should be a simple change in the post processor. Although it's also not retracting,

*************ignoring that, it's done in cycle, duuuuum moment.

Sent from my HTC One using Tapatalk

[Bm150]

Are you able to make a zip 2 go. If you can then I don't mind looking into it for you.

Sent from my HTC One using Tapatalk

[dougputt]

I'll try and zip the post. Thanks for your help!

[dougputt]

Not sure if this will work but here is zipped post

[Bm150]

Inside your zip is a .control file.
The file needed is a .pst file -should be in folder mill/posts.
cheers

[michael evans]

I think we had the same problem with our mazaks.. I will check on it...

[mactec54]

15 G20
N16 G0 G17 G40 G80 G90
N17 ( 1/8 SPOTDRILL TOOL - 4 DIA. OFF. - 4 LEN. - 4 DIA - .125 )
N18 ( DOUGS VMC 40 )
N19 ( CENTER )
N20 T4 M6
N21 A-0.
N22 G0 G90 S2139 M3 E11 X.5 Y4.5
N23G43 H4 Z2. M8
N24 G81 G98 X.5 Y4.5 Z-.1425 R0.1 F3.
N25 X3.5
N26 X.5 Y.5
N27 G80
N28 M5 M9
N29 G90 H0 Z0.
N30 M1
N31 ( .167 PILOT DRILL (21?) TOOL - 7 DIA. OFF. - 7 LEN. - 7 DIA - .167 )
N32 ( DOUGS VMC 40 )
N33 ( PILOT HOLE )
N34 T7 M6
N35 G0 G90 S1900 M3 E11 X.5 Y4.5
N36G43 H7 Z2. M8
N37 G83 G98 X.5 Y4.5 Z-.5602 R0.1 Q.0501 F2.74
N38 X3.5
N39 X.5 Y.5
N40 G80
N41 M5 M9
N42 G90 H0 Z0.
N43 M1
N44 ( .381 TIN DRILL BIT TOOL - 5 DIA. OFF. - 5 LEN. - 5 DIA - .381 )
N45 ( DOUGS VMC 40 )
N46 ( THROUGH HOLE )
N47 T5 M6
N48 G0 G90 S2406 M3 E11 X.5 Y4.5
N49G43 H5 Z2. M8
N50 G83 G98 X.5 Y4.5 Z-.7245 R0.1 Q.1143 F3.5
N51 X3.5
N52 X.5 Y.5
N53 G80
N54 M5 M9
N55 G90 H0 Z0.
N56 E0 X0 Y0
N57 M30
%
%

You have no G43 call in your program, this is the tool offset call without it you will crash, you need a G43 with each H1 for tool (1) for each tool change

[Bm150]

You have no G43 call in your program, this is the tool offset call without it it will crash, you need a G43 H1 for tool (1) at each tool change

It is there. Line 36

Sent from my HTC One using Tapatalk

[warrenb]

Don't know why it would make a difference but there is no space between the N## and the G43 Shouldn't matter but maybe it does.

[mactec54]

Bm150

I put them in there, look at the first posted code, it does not have any G43 tool offset call in the program

[mactec54]

Don't know why it would make a difference but there is no space between the N## and the G43 Shouldn't matter but maybe it does.

If you are using tool offsets, then you can not run the program without a G43 H---- tool number, without it you will crash, this is the very basics of programing

[Bm150]

Bm150

I put them in there, look at the first posted code, it does not have any G43 tool offset call in the program

Rodger that...

Sent from my HTC One using Tapatalk

[imdano]

shouldn't the end of program read:
G80
M5 M9
G90 G28 Z0.
X0. Y0.
M30

[mactec54]

dougputt

You will have to change the Z move at the end of each operation, this can be as simple as BM150 has already said

Instead of it being G90 H0 Z0. Which is incorrect, it needs to be G0G53Z0. You will have to see if the control will work without the G0 if it does, then all you need it to be G53Z0. this is all you need at the end of each tool operation

If you don't want the Z to go all the way home Z0 then you can give it a number like G0G53Z3. this will move the Z axes or tool 3" above the part, this number can be anything you want it to be, or were you want the Z axes to park after an operation

You can also use G0Z0. will do the same thing,

[dougputt]

dougputt

You will have to change the Z move at the end of each operation, this can be as simple as BM150 has already said

Instead of it being G90 H0 Z0. Which is incorrect, it needs to be G0G53Z0. You will have to see if the control will work without the G0 if it does, then all you need it to be G53Z0. this is all you need at the end of each tool operation

If you don't want the Z to go all the way home Z0 then you can give it a number like G0G53Z3. this will move the Z axes or tool 3" above the part, this number can be anything you want it to be, or were you want the Z axes to park after an operation

You can also use G0Z0. will do the same thing,

Thanks for all the input guys.
Mac I've been setting the Z0. to Z3. or something similar as mentioned, but what happens is it returns to Machine zero plus 3", it starts to drive tool down but by the time it hits the next line it starts to go to machine zero without the work offset. The fadal format 2 doen't use G43 codes I don't believe, or not with the Mcam post the way it is. It works fine for any tools that have a negative correction from my master tool.

[mactec54]

dougputt

I should of read what you posted better, did not see you were using a Fadal format 2, they have a positive & a negative tool offset G43 & a G44 for tool offset

Codes are attached

you can use these

G90 H0 Z0. You were missing the G0 in these lines G90 G0 H0 Z0

E0 X0 Y0

[dougputt]

Hi

I've removed the H0 cutter length cancel from lines 29 & 42 and seems to be work around for now. Just need to find it in the post...wonder what that will mess up..down the road..