4th axis post problem

[Stebedeff]

Hello there again,

I'am having some trouble with the post when using the rotary 4th axis ( x-axis).
I'am drilling holes on the top WCS and bottom WCS without a tool change.
Mastercam posts going from top to bottom all 4 axis's together and make my machine go on error cause it only takes 3 axis's at a time.
What I do to solve this is Force a Toolchange but this takes so much time.
Can someone help me solve this? Thanks




G21
G0 G17 G40 G49 G80 G90
( 10. SPOT DRILL | TOOL - 10 | DIA. OFF. - 10 | LEN. - 10 | TOOL DIA. - 8. )
( SPOT DRILL ALL HOLES TOP )
T10 M6
G0 G90 G54 X-8.452 Y18.126 U0. S2000 M3
G43 H10 Z100.
M8
G98 G81 Z-1.5 R5. F50.
X0. Y20.
X20. Y0.
X0. Y-20.
X-20. Y0.
G80
( SPOT DRILL HOLES 6MM )
G55 X-20. Y0. Z5. U0. <-------------------4 axis's
G99 G81 Z-1.7 R5. F50.
X0. Y20.
X20. Y0.
X0. Y-20.
G80
M9
M5
G91 G28 Z0.
G28 Y0. U0.
M30
%

[Superman]

This looks like Fanuc codes
Are you sure that your 4th axis is "U" ???

A is the designated rotary axis around X
B around the Y
C around the Z

U is normally an incremental linear axis parallel to X

Check your manuals

A0 should replace the 1st U0
A180 replace the 2nd U0

Another suggestion- try replacing G80 with G0 ( G80 on some machines forces the spindle to stop )

G21
G0 G17 G40 G49 G80 G90
( 10. SPOT DRILL | TOOL - 10 | DIA. OFF. - 10 | LEN. - 10 | TOOL DIA. - 8. )
( SPOT DRILL ALL HOLES TOP )
T10 M6
G0 G90 G54 X-8.452 Y18.126 A0. S2000 M3
G43 H10 Z100.
M8
G98 G81 Z-1.5 R5. F50.
X0. Y20.
X20. Y0.
X0. Y-20.
X-20. Y0.
G0
G91 G28 Z0. ( Clearance safe )
( SPOT DRILL HOLES 6MM )
G0 G90 G55 X-20. Y0. Z5. A180.
Z100.
G98 G81 Z-1.7 R5. F50.
X0. Y20.
X20. Y0.
X0. Y-20.
G0
M9
M5
G91 G28 Z0.
G28 Y0. U0.
M30
%

[Stebedeff]

Thanks for the quick reply.
Yes its a Fanuc. And the U is correct. I personaly don't know why the machine is set as "U" for a "A" axis but thats just how it is. G80 does not make my spindle stop. The program I just posted above is good. It's all about having 4 axis's programmed simultanously. The machine can only take 3axis's simultanously. I have this problem offten! I then just force toolchange so that the Z axis comes in the second line with G43 and H... This just takes much time cause the machine goes all the way back to machine zero.

[tobyaxis]

This looks a lot like a Lathe Post mixed with a Mill Post. I would call my Dealer to see if there was a mix up.

[Stebedeff]

It's not a mix. It's me who changed the post from A to U cause my machines 4th axis is a U instead of being a A.

[Superman]

oops

[Superman]

Let's put the U / A issue aside.

Your problem being, that your machine only interpolates 3 axes at any 1 time

The safest method is to break the Z moves. Travel in XYU to correct possition then descend in Z. When retracting, this is done in reverse order.

ie format
G21
G0 G17 G40 G49 G80 G90
( 10. SPOT DRILL | TOOL - 10 | DIA. OFF. - 10 | LEN. - 10 | TOOL DIA. - 8. )
( SPOT DRILL ALL HOLES TOP )
T10 M6
G0 G90 G54 X-8.452 Y18.126 U0. S2000 M3
G43 H10 Z100.
M8
G98 G81 Z-1.5 R5. F50.
X0. Y20.
X20. Y0.
X0. Y-20.
X-20. Y0.
G80
G91 G28 Z0. ( Clearance safe ) have this added for any rotate repositions
( SPOT DRILL HOLES 6MM )
G55 X-20. Y0. U0.
Z100.move the Z value down to next line
G99 G81 Z-1.7 R5. F50.
X0. Y20.
X20. Y0.
X0. Y-20.
G80
M9
M5
G91 G28 Z0.
G28 Y0. U0.
M30
%

Just an additional query , is V and W still incremental axes parallel to Y and Z ?
It is possible that a designated axis can have it's address reassigned to another letter. Is this possible?
That the letter has not been changed back
ie X and Y letters swapped is the same as rotating the part 90 degrees

[Stebedeff]

I have no idea of a V or W on a mill.
We just use X,Y,Z and U. Why a "U".
This because the machine parameter for 4th axis is set to letter U. I have a thread about changing the U back to A in the fanuc section but I guess no one could figure it out.
So in the workoffset page G54 to G59 I have a X,Y,Z and U axes.
I know it's confusing this U but I can't help it. We bought the machine second hand so that's just the way it is. And it works fine with mastercam except for the 4 axis's going simultaneously. This by the way only happens when I'am going to another machine WCS ( G54 to G59) using the same tool.
And changing the hole nc program might just take more time than programming the part itself when having lots of operations. I'am still a beginner in mastercam so I still make mistakes. So everytime I go and repost the nc program I don't feel like changing all the axis's again and again. I have been doing that in the beginning untill I got the curage of editing the post.
But I'am kind of out of luck with this one.
I've been looking through the post and changing stuff for days now but didn't get any good. I use/edit the standard Generic Fanuc 4x Mill.pst and tried the MPfan.pst but no luck.
I am very gratefull for all the help I got so far and would really like to get this fixed.

Thanks to all......

[Stebedeff]

To anyone having similar problems......
This is what you need to change in the post: Put the red colored pcout on a next line and ad a , e$ to it. Make sure it's on it's own line when editing. This will put the A axis on it's own line in the NC program.



ptlchg0$ #Call from NCI null tool change (tool number repeats)
pcuttype
pcom_moveb
c_mmlt$ #Multiple tool subprogram call
comment$
pcan
result = newfs(15, feed) #Reset the output format for 'feed'
pbld, n$, sgplane, e$
pspindchng
pbld, n$, scoolant, e$
if mi1$ > one & workofs$ <> prv_workofs$,
[
sav_absinc = absinc$
absinc$ = zero
pbld, n$, sgabsinc, pwcs, pfxout, pfyout, pfzout, pfcout, e$
pe_inc_calc
ps_inc_calc
absinc$ = sav_absinc
]
if cuttype = zero, ppos_cax_lin
if gcode$ = one, plinout
else, prapidout
pcom_movea
c_msng$ #Single tool subprogram call

--------------------------------------------------------------------------

ptlchg0$ #Call from NCI null tool change (tool number repeats)
pcuttype
pcom_moveb
c_mmlt$ #Multiple tool subprogram call
comment$
pcan
result = newfs(15, feed) #Reset the output format for 'feed'
pbld, n$, sgplane, e$
pspindchng
pbld, n$, scoolant, e$
if mi1$ > one & workofs$ <> prv_workofs$,
[
sav_absinc = absinc$
absinc$ = zero
pbld, n$, sgabsinc, pwcs, pfxout, pfyout, pfzout, e$
pfcout, e$
pe_inc_calc
ps_inc_calc
absinc$ = sav_absinc
]
if cuttype = zero, ppos_cax_lin
if gcode$ = one, plinout
else, prapidout
pcom_movea
c_msng$ #Single tool subprogram call


Thanks to all for helping!

[Superman]

Have you thought is right through

XYZ then U ??? would this not crunch on a 2nd op using the same tool at a different plane

IMHO it should be XYU then Z

if mi1$ > one & workofs$ <> prv_workofs$,
[
sav_absinc = absinc$
absinc$ = zero
pbld, n$,"G91 G28 Z0.", e$ #added
pbld, n$, sgabsinc, pwcs, pfxout, pfyout, pfcout, e$
pfzout, e$
pe_inc_calc
ps_inc_calc
absinc$ = sav_absinc

[Stebedeff]

Your Totally Right!!!
I was kind of stoked cause I finally found out how to change after lots of trying that I just post it right away before really checking it through how I want it. I put the U on second line and then the Z on one right after.

I even got through with the coolant how they should be.
Every thing was set with "scoolant" while it should be pcan, pcan1 and pcan2 for before, with and after. X style.
Deleted all the sequence numbers ( n$) except the ones in front of tool call.
so I get a N100 for firts operation and N200 for second and so on. I did learn a lot. I remember looking at a post the first time!!! I had no clue where to start or what was what. And now I know a little more so me too can help someone some day.


if mi1$ > one & workofs$ <> prv_workofs$,
[
sav_absinc = absinc$
absinc$ = zero
pbld, n$,"G91 G28 Z0.", e$ #added
pbld, n$, sgabsinc, pwcs, pfxout, pfyout, e$
pfcout, e$
pfzout, e$
pe_inc_calc
ps_inc_calc
absinc$ = sav_absinc


Thanks.....