Live tooling spindle direction

[Zoffen]

Hello all emastercamers!

 

I am having problem getting my live tools to spin the right direction.

 

If i use a cross direction, i.e. a radial live tool, front,bac,ect. it outputs a code to start the spindle backwards, while if i use a axial live tool with the right plane it will start the spindle the proper direction. Can anyone tell me how to fix this so i don't smoke anymore tools?

thanks a bunch!

[uncle_dolan]

Does modifying your spindle direction in the tool setup parameters change it?

[Zoffen]

Does modifying your spindle direction in the tool setup parameters change it?

I can use the same tool and it can be set to CW for an axial operation and a radial operation and the radial will give a CCW code and the Axial will give a CW code.

[uncle_dolan]

I've only used live tooling on a lathe that had actual interface programming, and it would do the same thing so we just had to tell it that the tool was meant to rotate the other direction. It only did it on some of our holders though ( I think the 4x RPM multiplier holders) and not on the 16x multipliers... Not sure how to manage this in mastercam. There may be something that you have to set up in the machine definition to manage this, but again, my experience with those tools are limited to controller based programming. Hope this helps anyway. brendan

[Russh67]

Hello all emastercamers!

 

I am having problem getting my live tools to spin the right direction.

 

If i use a cross direction, i.e. a radial live tool, front,bac,ect. it outputs a code to start the spindle backwards, while if i use a axial live tool with the right plane it will start the spindle the proper direction. Can anyone tell me how to fix this so i don't smoke anymore tools?

thanks a bunch!

 

I've had this problem.

 

Our machine; spindle on left tools on right in the back. when milling or drilling, ect live tools on the front face facing the spindle we need to command an M74 (live tools spindle CCW), When milling or drilling live tools on the side we need to command M73 (live tools spindle CW). This will make the tools climb as the should.

 

My post posts an M73 for all live tools.

 

I note the Tool Number that need changing and change manually in the program. It's a little bit of a pain...

 

I like you, would love to have the post do this automatically...

[Russh67]

Hello all emastercamers!

 

I am having problem getting my live tools to spin the right direction.

 

If i use a cross direction, i.e. a radial live tool, front,bac,ect. it outputs a code to start the spindle backwards, while if i use a axial live tool with the right plane it will start the spindle the proper direction. Can anyone tell me how to fix this so i don't smoke anymore tools?

thanks a bunch!

 

 

What kind of live tools are you using??

 

 

I've had this problem.

 

Our machine; spindle on left tools on right in the back. when milling or drilling, ect live tools on the front face facing the spindle we need to command an M74 (live tools spindle CCW), When milling or drilling live tools on the side we need to command M73 (live tools spindle CW). This will make the tools climb as the should.

 

My post posts an M73 for all live tools.

 

I note the Tool Number that need changing and change manually in the program. It's a little bit of a pain...

 

I would love to have the post do this automatically...

[Josh Kinney -Elite Engineering]

My InHouse NL2500 post outputs M13 or M14 depending on Face or Radial. Sounds like you just need to switch the direction codes in the post.

[Colin Gilchrist]

What Post are you using?

 

In the Generic Fanuc 4X MT_Lathe Post, there is a series of strings that control the setup for code output, based on what kind of cut (cross/face) is active.

 

This is the 'scase' series of strings.

 

For Cross Cuts (live tool perpendicular to the lathe spindle), you would need to modify the 'scase_tl_c3' line.

 

scase_tl_c3  : "10010102.000000000"  #Top turret/Left spindle, Cross cut

Changing the 2nd parameter from '0' to '1' should reverse the spindle direction for Cross cutting:

 

scase_tl_c3  : "11010102.000000000"  #Top turret/Left spindle, Cross cut

[Josh Kinney -Elite Engineering]

That's great info. Thanks Colin!

[Colin Gilchrist]

If you look above the 'scase' section in the PST file, there are some comments that describe what each of those digits does. There is also a section directly above the 'scase'settings that control the position output for Cutter Compensation codes during Lathe Canned Cycles.

 

Here is the entire section I'm referring too:

 

# --------------------------------------------------------------------------------------
#Lathe canned turning settings:
#
# Set each digit of slcc_options to 0 or 1 to activate the proper canned cycle format 
# based on where your machine expects the cutter comp codes for Lead in/out moves.
#
# The default value of slcc_options ("0010000100") will output the Cutter Comp codes 
# inside the canned cycle. This maintains compatibility with Pre-X5 posts.
#
# To output the Cutter Comp codes outside the macro, un-pound the line for the second 
# slcc_options, and comment out the first option. 
# --------------------------------------------------------------------------------------
lcc_mov_mult : 2.    #Enter the move radius multiplier in X, Z for lathe canned cycle comp.

# A - Pattern, Rough, Comp lead addition, dependent on B
# B - Pattern, Rough, Comp before/after cycle
# C - Pattern, Rough, Comp in profile
#
# D - Pattern, Finish, Comp lead addition, dependent on E
# E - Pattern, Finish, Comp before/after profile
#
# F - Face/Turn, Rough, Comp lead addition, dependent on G
# G - Face/Turn, Rough, Comp before/after cycle
# H - Face/Turn, Rough, Comp in profile
#
# I - Face/Turn, Finish, Comp lead addition, dependent on J
# J - Face/Turn, Finish, Comp before/after profile

#Columns-       ABCDEFGHIJ    #Comp Output
slcc_options : "0010000100"   #Pattern & Face/Turn inside Canned Profile
#slcc_options : "1101111011"  #Pattern & Face/Turn outside Canned Profile

# --------------------------------------------------------------------------
#Machining position turret/spindle settings
# Switch strings based on turret position top/bottom-left/right and cut type.
# Turret position is based on the Mastercam settings (see lathtype).
# Strings are re-assigned for output in the routine psw_str_mult.
# The string variable sw_string holds the place position value to determine
# how to assign the strings.  Planes are relative to the view from Mastercam.
# Assign the 17 digit string following the alpha columns below:
# A - C axis, 1 = axis winds, 2 = axis signed, 3 = indexer, 4 = shortest direction
# B - Spindle direction, 0 = normal, 1 = reverse
# C - Plane 0 arc/comp, 0 = normal, 1 = switch
# D - Plane 1 arc/comp, 0 = normal, 1 = switch
# E - Plane 2 arc/comp, 0 = normal, 1 = switch
# F - Plane 0, 0 = G17, 1 = G19, 2 = G18
# G - Plane 1, 0 = G17, 1 = G19, 2 = G18
# H - Plane 2, 0 = G17, 1 = G19, 2 = G18
# Decimal (required)
# I - Plane 0, X axis, 0 = normal, 1 = switch sign from basic
# J - Plane 0, Y axis, 0 = normal, 1 = switch sign from basic
# K - Plane 0, Z axis, 0 = normal, 1 = switch sign from basic
# L - Plane 1, X axis, 0 = normal, 1 = switch sign from basic
# M - Plane 1, Y axis, 0 = normal, 1 = switch sign from basic
# N - Plane 1, Z axis, 0 = normal, 1 = switch sign from basic
# O - Plane 2, X axis, 0 = normal, 1 = switch sign from basic
# P - Plane 2, Y axis, 0 = normal, 1 = switch sign from basic
# Q - Plane 2, Z axis, 0 = normal, 1 = switch sign from basic
use_only_tl  : 1     #Use only Top turret/Left spindle settings (below) for
                    #all Mastercam turret/spindle selections
                    #When configuring for multi-spindle/turret set to 0

#Columns-       ABCDEFGH.IJKLMNOPQ #Turret/Spindle            #Path Type
scase_tl_c1  : "10000222.000000000"  #Top turret/Left spindle, Turning cut
scase_tl_c2  : "11000012.000000000"  #Top turret/Left spindle, Right Face cut
scase_tl_c_2 : "11110012.000000000"  #Top turret/Left spindle, Left Face cut
scase_tl_c3  : "10010102.000000000"  #Top turret/Left spindle, Cross cut
scase_tl_c4c : "10000111.000000000"  #Top turret/Left spindle, Y axis subs. Cycle
scase_tl_c4  : "10000222.000000000"  #Top turret/Left spindle, Y axis subs.
scase_tl_c5  : "10000222.000000000"  #Top turret/Left spindle, Multisurf Rotary

#Columns-       ABCDEFGH.IJKLMNOPQ
scase_bl_c1  : "10000222.000000000"  #Bottom turret/Left spindle, Turning cut
scase_bl_c2  : "11000012.000000000"  #Bottom turret/Left spindle, Right Face cut
scase_bl_c_2 : "11110012.000000000"  #Bottom turret/Left spindle, Left Face cut
scase_bl_c3  : "10010102.000000000"  #Bottom turret/Left spindle, Cross cut
scase_bl_c4c : "10000111.000000000"  #Bottom turret/Left spindle, Y axis subs. Cycle
scase_bl_c4  : "10000222.000000000"  #Bottom turret/Left spindle, Y axis subs.
scase_bl_c5  : "10000222.000000000"  #Bottom turret/Left spindle, Multisurf Rotary

#Columns-       ABCDEFGH.IJKLMNOPQ
scase_tr_c1  : "10000222.000000000"  #Top turret/Right spindle, Turning cut
scase_tr_c2  : "11000012.000000000"  #Top turret/Right spindle, Right Face cut
scase_tr_c_2 : "11110012.000000000"  #Top turret/Right spindle, Left Face cut
scase_tr_c3  : "10010102.000000000"  #Top turret/Right spindle, Cross cut
scase_tr_c4c : "10000111.000000000"  #Top turret/Right spindle, Y axis subs. Cycle
scase_tr_c4  : "10000222.000000000"  #Top turret/Right spindle, Y axis subs.
scase_tr_c5  : "10000222.000000000"  #Top turret/Right spindle, Multisurf Rotary

#Columns-       ABCDEFGH.IJKLMNOPQ
scase_br_c1  : "10000222.000000000"  #Bottom turret/Right spindle, Turning cut
scase_br_c2  : "11000012.000000000"  #Bottom turret/Right spindle, Right Face cut
scase_br_c_2 : "11110012.000000000"  #Bottom turret/Right spindle, Right Face cut
scase_br_c3  : "10010102.000000000"  #Bottom turret/Right spindle, Cross cut
scase_br_c4c : "10000111.000000000"  #Bottom turret/Right spindle, Y axis subs. Cycle
scase_br_c4  : "10000222.000000000"  #Bottom turret/Right spindle, Y axis subs.
scase_br_c5  : "10000222.000000000"  #Bottom turret/Right spindle, Multisurf Rotary

[Zoffen]

Thanx for the info colin!

[Colin Gilchrist]

Thanks guys, I hope it helps...

[Josh Kinney -Elite Engineering]

Colin,

This works great, got my main spindle (Upper Left) outputting M14 and my Sub Spindle (Upper Right) outputting M13 like it should. Now I need it to output a M245 for the Sub instead of a M45. How can I do this? How does it decide between *sm24 and *sm224/ *sm23 *sm223?

 

Thanks,

 

Josh-

[Josh Kinney -Elite Engineering]

Can anybody help?

 

I need to get this last bit worked out.

 

Thanks,

 

Josh-

[Guest CNC Apps Guy 1]

Some Right Angle mfrs have their gearing set up so that forward is forward and backward is backward.

 

I like those.

[crazy^millman]

Josh, for sub splindle you will need to work out the spindle logic in your post. The post Colin is referring to has a spindle_no$ this is what tells the post if you are using the main or the sub spindle. So you need to work out the logic that is the main spindle is called on the these codes get called and if the sub splindle is called then these codes get called.

 

Looks like the post Colin is talking about handles M23 here:

 

pcaxis_on_m 	#Toolchange C axis enable, mill, check prv_ to current
 	if (rc1 = two | prv_posttype$ = two),
   	[
   	pbld, n$, *sm23, e$
   	if nextdc$ = three, pbld, n$, "M49", e$  #Disable tap
   	]

then handles M24 here:

 

#Rc1 is used to flag the SOF, rc1 = two at SOF
pcaxis_off_l	#Toolchange C axis disable, lathe, check prv_ to current
 	if rc1 > two & prv_posttype$ <> two, pbld, n$, *sm24, e$

So I think this is real easy to fix:

 

Look for the sm23 and sm24 section and add the sm223 and sm224 now you can name these anything you want as long as you do not duplicate something already defined in the post.

 

# --------------------------------------------------------------------------
# C axis mode
sm23	: "M23"  	#C axis enable main spindle
sm24	: "M24"  	#C axis disable main spindle
sm223 : "M224"	#C axis enable sub spindle
sm224 : "M224"	#C axis disable sub spindle

Add the logic of the spindle_no$ and you are pretty much done.

 

pcaxis_on_m 	#Toolchange C axis enable, mill, check prv_ to current
 	if (rc1 = two | prv_posttype$ = two),
   	[
   	if spindle_no$ = 0, pbld, n$, *sm23, e$
   	if spindle_no$ = 1,pbld, n$ *sm223, e$
   	if nextdc$ = three, pbld, n$, "M49", e$  #Disable tap
   	]


#Rc1 is used to flag the SOF, rc1 = two at SOF
pcaxis_off_l	#Toolchange C axis disable, lathe, check prv_ to current
 	if spindle_no$ = 0, if rc1 > two & prv_posttype$ <> two, pbld, n$, *sm24, e$
 	if spindle_no$ = 1, if rc1 > two & prv_posttype$ <> two, pbld, n$, *sm224, e$

 

This is not tested so use at your own risk, but I think it should be on the right track. I do not think you need to bracket the condition statements.

 

Colin can you see about getting sub spindle support for these type of codes added to the generic post you referenced. I am surprised it is not already built in. Thanks

 

HTH

[Josh Kinney -Elite Engineering]

Thanks for that info. I'm using the inhouse post and it has that logic. Problem is when milling the only way to tell the post your on the side is "Left View" and "Upper Right Turret".

 

I could have it check for which side of the turret?

 

Josh-

[Ron Branch @ 5th Axis]

Dohhhhhhhhhhhhhhh

[crazy^millman]

Yes there is turret logic as well or you could use a mi or mr to control it.

[Josh Kinney -Elite Engineering]

I'm assuming it knows that it's pltype3 based on the "Upper Right" turret specified in my Sub Spindle Milling Op. I'm also assuming it's something that needs changed in the corresponding post block.

 

pltype3 #Top turret/Right spindle

if cuttype = one,

[

#Lathe

max_speed = max_speedl3

min_speed = min_speedl3

sw_string = scase_tr_c1

]

else,

[

#Mill

max_speed = max_speedm3

min_speed = min_speedm3

sw_string = scase_tr_c2 #case two is the default

if cuttype = -2,sw_string = scase_tr_c_2

if cuttype = three, sw_string = scase_tr_c3

if cuttype = -3, sw_string = scase_tr_c3r

if cuttype = four & abs(c1_millcc) = one, sw_string = scase_tr_c4c

if cuttype = four & c1_millcc = zero, sw_string = scase_tr_c4

if cuttype = five, sw_string = scase_tr_c5

]

[Josh Kinney -Elite Engineering]

It's not there. I had a section that was forcing the output to be M45/M245. Now I have this

 

if not (livetool_flg),

[

if spindle_no$ = 0, pbld, n$, sm23, , e$

if spindle_no$ = 1, pbld, n$, sm223, , e$

livetool_flg = 1

]

 

Thanks guys!

 

Josh-

[crazy^millman]

No I am thinking then it goes back to lathtype in the code call then. Those are just settings to control moves and direction calls and items like that, for the M calls you are looking at goes back to the sections they are called from they control the call so the logic for them is where I would look first. If not sure always run the debugger in run mode not turbo and see every line called to know what is calling what where and when. This should help you narrow it down real quick.

[crazy^millman]

Okay you figured it out as I was typing my last response. Glad it worked out and thanks for sharing what got it working.

[Josh Kinney -Elite Engineering]

All fixed. I didn't see the forced output for live tooling. This is a modified mplmaster post. Works like a charm now!

[crazy^millman]

Crazy concept a post that outputs all the codes you need without hand editing. That is crazy I tell you.