makino question

[DF1]

to all makino and mastercam users,this is my first post so forgive me if it makes no sense

we are running mastercam x9 and are currently awaiting delivery of a makino f3,it comes with the die mold package, nano smoothing and sgi4.

I am currently using fanuc based mills but not to the makino level.

I will be milling copper electrodes and hardened cores and cavities for mold making

I have a few questions

1.how do you output sgi codes(ie m250 m251 etc)with the various toolpaths,do you do this with misc integers

   is it possible to have roughing toolpaths(ie optirough,area clearance,2d high speed) output m251 roughing code automatically.

2.does the makino run better with filtered toolpaths or point to point code,does sgi run with filtered toolpaths

3.our reseller is looking for info for a post, to turn on the sgi is the below format correct is there any thing missing

   .O0001 (ELE2F)
    ( 12 ML RIPP  -  CUTTER DIA 12. )
    ( SURFACE HIGH SPEED - AREA CLEARANCE)
    ( R.20  F.15 )
    N2 G21
    N4 G0 G17 G40 G49 G80 G90
    N8 T1 M06
    N10 T7
    N12 G0 G90 G54 X-22.152 Y-17.824 S8000 M3
    N14 G43 H1 Z10. M8
    N16 M251   ====================================is this all I need to turn sgi on
    N18 Z.5
    N20 G1 Z-1.626 F2000.
    N22 X-22.178 Y-17.835 Z-1.96

4.we usually call our programs by name(ie ele1r,ele1f etc)I think the makino needs to be called O0001,can the makino run progs other than O0000.

if it has to be O0001 how do most of you handle posting many different programs at a time,we are mold makers so programs are only usually ran once.
   any help would be much appreciated.

also can any one show me what the start of a prog shuold look like.our mastercam reseller is looking for this to get a post sorted out

 

 

 

 

 

 

 

[Bob W.]

It sounds like you have the Pro5 control.  Here are the answers to the best of my ability.

 

1.  Correct, M250 is standard mode, M251 is roughing and M252 is high accuracy I believe.  I'm not sure on M252 because standard mode has always been good enough for what we do.  I modified my post so these can be activated by misc integers and I believe the post can be modified to do it automatically.  These can also be changed mid-program (mid tool path) in the function menu if the machine isn't running smoothly.  Sometimes it gets going so fast I fear it might shake itself apart so I change the mode.

 

2.   Makinos with SGI.4 run better point to point with small moves.  I typically set my tolerance to .0002", turn on smoothing, present arcs as lines, and set the move length to .005-.010 depending on geometry.

 

3.  No issues jumped out at me.

 

4.  I assume you have the data server?  If so you can run from DNC with standard names (widget.NC, etc...).  Any programs called via M198 need to be in O0001 format.

[Bob W.]

I need to clarify that I only run point to point when finishing, not roughing.  When roughing I run filtered toolpaths with arcs on.

[DF1]

Thank you for your reply,it has the pro5 control,20000 rpm Hsk a63,and we are tooling with a combination of shrink fit and hydraulic chucks

[DF1]

Bobw,when you rough with arcs filtered toolpaths does the sgi preform correctly,was talking to someone and they told me that when you use arcs that the control processor needs to calculate more and this slows down the sgi performance,do you arc filter the toolpaths and post the out as point to point with your post

[Zoober]

Gimme a bit Df1. We have F5's and I've got it set up with Mi's for sgi. 4. Same machine, only biggerer. I'll post up some samples.

[Bob W.]

Bobw,when you rough with arcs filtered toolpaths does the sgi preform correctly,was talking to someone and they told me that when you use arcs that the control processor needs to calculate more and this slows down the sgi performance,do you arc filter the toolpaths and post the out as point to point with your post

I don't really notice but posting roughing point to point makes the programs huge which slows down Mastercam verify and Vericut.  That is the main reason I rough with arcs.  Also, the moves need to be really small or the servos will make some noise and the machine will not run smoothly, at least that is my experience.  I am running A51nx HMCs.  For finishing you absolutely should run point to point.

[Zoober]

As Bob says with the filtering and Dataserver. Big programs should be run from there with M198Pxxxx due to storage.

Make a simpple main to call the big toolpath sub.

Points not arcs. SGI.4 loves points. The more the better.

M250 = High Accuracy

M251 = high performance - fastest, least accurate

M252 = Ultra High Accuracy - slowest, most accurate.

M253 = Special with Rotary

 

Here is how I set using Misc reals...

 I have the phsm postblocks to turn on and off that I call in various places like ptolchg, ptlchg0, pretract, etc.

 

phsm1_on         #SGI 4 High speed functions before G43
      if mr1$ = 0, mr1$ = 2

      if mr1$ = 1 & mr1_flg <> 1,
        [
        pbld, n$, "M250", e$

        mr1_flg = 1
        ]
      if mr1$ = 2 & mr1_flg <> 2,
        [
        pbld, n$, "M251", e$

        mr1_flg = 2
        ]
      if mr1$ = 3 & mr1_flg <> 3,
        [
        pbld, n$, "M252", e$

        mr1_flg = 3
        ]
      if mr1$ = 4 & mr1_flg <> 4,
        [
        pbld, n$, "M253", e$

        mr1_flg = 4
        ]

phsm_off    #No off function for SGI 4?    
      if mr1_flg = 1,
        [

        mr1_flg = 0
        ]
      if mr1_flg = 2,
        [

        mr1_flg = 0
        ]
      if mr1_flg = 3,
        [

        mr1_flg = 0
        ]
      if mr1_flg = 4,
        [

        mr1_flg = 0
        ]

[Zoober]

Samples...

O2541 (102541)
(PGM P11111)
()
(OPERATION 70)
(FIXTURE - PROTOTYPE JAWS)
(MAKINO F5)
(RKB 11/30/15)




G00 G17 G20 G40 G80 G90
N10(A0 - RGH 11.1 DEG ANGLE)
G90
T1(1/4 R.015 6 FLT T-CARB EM)
M6
M11
G00 G17 G90
G54.1 P1 A0. X-1.4617 Y-3.1397 S4966 M03
M10
M251
G43 H1 Z2.125 M08
T2
G90 Z.225
G01 Z-.25 F30.
G41 D17 X-1.6089 Y-3.111 F35.7
X-1.6368 Y-3.2537

....

...

...

 

G00 Z2.125
(A0 - RGH .190 DIM FLAT AND 11.1 DEG ANGLE)
X-1.5223 Y-2.9174
M251
Z.225
G01 Z-.25 F30.
G41 D17 X-1.6723 F35.7
Y-2.9374
Y-3.2121
G02 X-1.6755 Y-3.2461 I-.1775 J0.
G01 X-1.7212 Y-3.48
X-1.7306 Y-3.5279
X-1.7421 Y-3.5868
G40 X-1.5949 Y-3.6155

....

....

....

 

 

N20(A-90 - RGH SMALL VEE POCKET)
G90
T2(.031 R.005 4 FLT RGH EM )
M6
M11
G00 G17 G90
G54.1 P2 A-90. X-1.8401 Y.0478 S18483 M03
M10
M251
G43 H1 Z4.47 M08
M26
T3
G90 Z3.57
G01 Z3.4236 F32.
X-1.8449 Y.0505 F26.
G03 X-1.8484 Y.0515 I-.00346 J-.00606
G01 X-1.8496

[DF1]

Thank you zoober,i don't know how to edit posts,our mastercam reseller does All our post edits.i see on your image on mi's that you have an option sgi 0=off,I didn't know that it could be turned off.iff you turn it off how does the mill preform is it just like a basic mill.

It seems to be your standard fanuc post and add the sgi codes before the nc code.we have roders hsm and there is so much more to look out for

 

So when machine arrives I'll rough with arcs and m251

And finish point to point with m250 or m252

[DF1]

Zoober do you turn sgi off for drilling operations

[Zoober]

You really can't turn it off. In the post, if you set it to sgi = 0, then it makes it M251. I did that to make it revert to M251 if it wasn't set at all, as in a drill cycle.

I don't want it drilling if the previous setting was ultra accurate, and forget to set it back.

 

From above:

phsm1_on         #SGI 4 High speed functions before G43
      if mr1$ = 0, mr1$ = 2

[betts]

Zoober I notice you are using the default "H1" for all tool heights, but not the D2, is there a reason for that?  We have always run "H1 D2" spit at all tlchg with the G43 and it was a big help when moving into pallet systems.  With DF1 only having the one machine for now I don't know if it will matter to him, but thought I would mention.

 

Another thing; for all of our 4-axis we had (still are) spitting out the M10/M11 all the time except full four movement.  Going to 5-axis we picked up a post from a sister company and they were running unlocked all the time.  When we talked to Makino about it they swear there is more torque when running unlocked and they recommend just running unlocked all the time.  Anyone have input one way or the other on that?  All the 5-axis are rotary/rotary.

[Zoober]

The reason for the H1 D17 is simply consistency. When I got here, our existing A61's (pro 3) were set up for H1 D17. Not sure why, but I had Makino set up our new F5's (pro 5) the same way for consistency. The D17 (or D whatever) just subs out to the Makino Tool Data from the Fanuc side.

No other reason. You could make it anything you want to fit your needs. Many machines use D99 for their calls to the tool manager.

These are verticals with Tsudakoma 4th rotaries. I would not run them unlocked unless (obviously) for full 4th.

Some Horizontals automatically lock/unlock on B moves. Niigata is that way. you must explicitly unlock them for full 4th.

But I would definitely trust the builder (especially one of Makino caliber) over me any day.

[Sticky]

 

Another thing; for all of our 4-axis we had (still are) spitting out the M10/M11 all the time except full four movement.  Going to 5-axis we picked up a post from a sister company and they were running unlocked all the time.  When we talked to Makino about it they swear there is more torque when running unlocked and they recommend just running unlocked all the time.  Anyone have input one way or the other on that?  All the 5-axis are rotary/rotary.

 

Unless you are hearing this from a mechanical engineer at Makino (not a service guy, and not an apps guy) I would be skeptical. The drive method of the rotary axis really matters here, if it is a worm drive, then lock is always going to be the best method. If you don't then the worm wears un-evenly on all your common indexes, which then creates problems for the times you do need full contouring. Direct drive is a different ballgame, even then, most builders still use a mechanical brake, and if they do then it would be better to use that, so you aren't putting as much strain on the motor and drive.

[Bob W.]

Another thing; for all of our 4-axis we had (still are) spitting out the M10/M11 all the time except full four movement.  Going to 5-axis we picked up a post from a sister company and they were running unlocked all the time.  When we talked to Makino about it they swear there is more torque when running unlocked and they recommend just running unlocked all the time.  Anyone have input one way or the other on that?  All the 5-axis are rotary/rotary.

Are these direct drive?  If so DO NOT run unlocked.  When the DD can't handle the torque (roughing) it simply lets go completely.  Ask me how I know...  I took their advice and had it let go twice in two weeks and I changed back.  It was a huge mistake and scrapped an expensive indexable cutter in the process.  If you run high speed machining and put any load on the machine you are playing with fire if you run unlocked.

[mkd]

Are these direct drive?  If so DO NOT run unlocked.  When the DD can't handle the torque (roughing) it simply lets go completely.  Ask me how I know...  I took their advice and had it let go twice in two weeks and I changed back.  It was a huge mistake and scrapped an expensive indexable cutter in the process.  If you run high speed machining and put any load on the machine you are playing with fire if you run unlocked.

I ran a production job on a NH4000DCG (direct drive) where we made 30,000 complex buttstock parts in under a years time.

 i ran lock/unlock on every index...

..

..

until the brake piston seal let go.

 from then on i only clamped for heavy cutting.

[betts]

 

 

Are these direct drive?  If so DO NOT run unlocked.  When the DD can't handle the torque (roughing) it simply lets go completely.  Ask me how I know...  I took their advice and had it let go twice in two weeks and I changed back.  It was a huge mistake and scrapped an expensive indexable cutter in the process.  If you run high speed machining and put any load on the machine you are playing with fire if you run unlocked.

 

We still run the a61's (Makino's with the lock/unlock unless the path is full 4, but the a51's and a82 are running unlocked all the time.  Those machines run only aluminum so while you can still pull some horses it would be more concerning if we were running something tougher.  The a51's and a82 are 5-axis with a Koma rotary.

 

So when you switched to running locked on roughing, did you set this up in Misc Integers or hand edit?  We have changed the posts for the conditions we want, which in the case of the a61's is all the time except full 4 motion.

[Bob W.]

We still run the a61's (Makino's with the lock/unlock unless the path is full 4, but the a51's and a82 are running unlocked all the time.  Those machines run only aluminum so while you can still pull some horses it would be more concerning if we were running something tougher.  The a51's and a82 are 5-axis with a Koma rotary.

 

So when you switched to running locked on roughing, did you set this up in Misc Integers or hand edit?  We have changed the posts for the conditions we want, which in the case of the a61's is all the time except full 4 motion.

I just hard coded it in my posts.  I think the best method would be for the post to detect the nature of the toolpath and control the lock/ unlock automatically.  That would be the best of both worlds.  How difficult would it be to detect the following toolpaths and set them to lock and leave everything else open?

 

Opti-rough

Opti-rest

2D HST - dynamic, peel, etc...

3D HST area clearance

Facing

 

Ones left off would be drilling, tapping, contouring, standard pocketing, surfacing, etc...  I know on my machines it would be a time saver to not always lock and like MKD pointed out, it would suck to wear out a seal and have a machine down.

[Sticky]

How long does the lock on your guys Makino's take? My Matsuura's lock in about a half second. There are better places to shave time imo.

[betts]

I don't even think it takes a half second, it isn't really a time thing.  It was more of a PITA just getting the post dialed in for all the possible combinations.  Unless we are missing something in the parameters the machine will not throw an alarm when the B is locked and you invoke a B rotation.  So if you have it locked and it comes to a B command it just sits there not moving and doesn't tell the operator anything.

[crazy^millman]

Well with a good post I have never seen that problem. Once the post gets dialed in then you are golden.

[mkd]

I just hard coded it in my posts.  I think the best method would be for the post to detect the nature of the toolpath and control the lock/ unlock automatically.  That would be the best of both worlds.  How difficult would it be to detect the following toolpaths and set them to lock and leave everything else open?

 

Opti-rough

Opti-rest

2D HST - dynamic, peel, etc...

3D HST area clearance

Facing

 

Ones left off would be drilling, tapping, contouring, standard pocketing, surfacing, etc...  I know on my machines it would be a time saver to not always lock and like MKD pointed out, it would suck to wear out a seal and have a machine down.

nice!

 could turn it into a whole section in the .pst file where users can pre select which ops will automatically lock B.

Misc integers for the odd large drilling operation/ when the need arises.

[Jayson Kramer]

For the Makino I am programming for the post like zoober is set with the options so code looks like this.

(TIME      - 1:59 PM)
(N1 - T1 - 3/4 ENDMILL .03R     - H1 - D17)
G91 G00 G30 Z0.
N1 G00 G80 G17 G40 G98 G91 G30 M09 Z0.
M11 (UNLOCK B )
G90 B0.
M10 (LOCK B )
(3/4 ENDMILL .03R)
(ROUGH RIGHT SIDE)
(OPERATION NO - 6)
(TOOLPATH - AREA CLEARANCE...)
(STOCK LEFT ON WALLS = .01)
(STOCK LEFT ON FLOORS = .01)
T1 M06
G00 G54 G17 G90
M26
S13242 M03
M11 (UNLOCK B
G90 G00 B90.
G00 G91 B5.
G01 G91 B-5. F100.
G00 G90
M10 (LOCK B )
M251
G05.1 Q1
G00 G90 G54 X-3.01363 Y-1.49407
G43 H1 Z6.
Z4.4025
G94 G01 Z2.9925 F300.
Z2.9175
X-2.86081 Y-1.12457 Z2.90939 F397.26
X-2.85826 Y-1.03537 Z2.9075
G03 X-3.16302 Y-.97716 I-.31422 J-.81826

This works well.

[DF1]

thanks jay.

thank you all for your replys.

we wont have a rotary axis on our machine. we are expecting delivery in the next 2 weeks so I am trying to get as much

info together for my reseller to get a post sorted out for training. our reseller can be a bit on the slow side when it comes to modifying a post and I don't want to much left  to be done as the training starts.

i have asked our makino man for the pro5 programming guide on pdf but he says he is not allowed to give out pdf versions of the manuals.

am I correct in saying the tool offsets can be on both fanuc side and makino side.if so why is this and what are the advantages of both.we are mold toolmakers so which would be

best for us.we usually run only one or two of any of our programmes(ie.electrodes)

jay could you put up a screen shot of your misc int page.after the M251 you have "G05.1 Q1"(super sgi mode on) do you have this on your misc int page also or is it coded to your post when you call a sgi code. 

also for a machine like this do any of you set the "chordal deviation" in your MDCD to a finer setting than default.(mine is currently set to 0.01mm),but it is fine for the machine im on at the moment.

I will be doing mostly 3d machining on copper electrode and hard steel