Need 5-axis post help

[Bob W.]

I am currently working on adapting the generic Fanuc 5-axis post to work with my machine which is a Makino A51 horizontal machine with a rotary table. I have my machine set up like a vertical, meaning I program it how I would program a vertical and I need to create planes for the b-axis 90 and -90 degree indexes. I have things pretty well dialed in but when my test program goes to make a 5-axis swarf cut the C axis is off by 90 degrees. Anyone know what setting I need to change to fix this? I have another working post that does this correctly but it has so many other issues I felt it would be better to start from scratch and adapt a new post. I am doing all of my testing in Vericut.

 

Another issue I get with both posts if minimum feed rate outputs in various locations. My machine takes inverse feed rates up to 999999. and there are some pretty tight moves that are feeding in the 150000 range. Randomly there will be feed rates of 500, which is the default minimum set in the post and it causes the machine to run very rough with a lot of dwells.

[Bob W.]

Got the 90 degree offset fixed with the help from Colin Gilchrist. Thanks a ton Colin, I really appreciate it. I still have the issue of the minimum feed randomly appearing though. These are moves that should be in the 150000. range so they are very out of place. Also, is there a way to force the post to output X,Y,Z,B,and C, and the feed on every line for full 5-axis surfacing? I was told by Makino that this is what the control likes to be fed and it works better this way with the SGI.

[Bob W.]

The feed issue appears to be directly related to the tolerances set in the control definition. The feeds are output correctly with looser tolerances and when they are tightened up the feed issues appear. Any idea what these tolerances should be set to? The post refers to a NCI tolerance that should be set to the 7th decimal place but I can't find it anywhere in any of the configuration fields. Also, this is only outputting to the 4th decimal place for linear moves and I would like it to output the 5 that the machines will accept. Where is the setting that controls this?

[Jeremy Herron@DBS Solutions™]

As far as decimal output this should do it...

 

# Format statements - n=nonmodal, l=leading, t=trailing, i=inc, d=delta

# --------------------------------------------------------------------------

#Default english/metric position format statements

fs2 1 0.7 0.6 #Decimal, absolute, 7 place, default for initialize ( : )

fs2 2 0.5 0.4 #Decimal, absolute, 4/3 place

fs2 3 0.4 0.3d #Decimal, delta, 4/3 place

#Common format statements

fs2 4 1 0 1 0 #Integer, not leading

fs2 5 2 0 2 0l #Integer, force two leading

fs2 6 3 0 3 0l #Integer, force three leading

fs2 7 4 0 4 0l #Integer, force four leading

fs2 8 5 0 5 0l #Integer, force five leading

fs2 9 0.1 0.1 #Decimal, absolute, 1 place

fs2 10 0.2 0.2 #Decimal, absolute, 2 place

fs2 11 0.3 0.3 #Decimal, absolute, 3 place

fs2 12 0.4 0.4 #Decimal, absolute, 4 place

fs2 13 0.5 0.5 #Decimal, absolute, 5 place

fs2 14 0.3 0.3d #Decimal, delta, 3 place

fs2 15 0.2 0.1 #Decimal, absolute, 2/1 place

fs2 16 1 0 1 0n #Integer, forced output

fs2 17 1.4 1.3lt #Decimal, absolute, 4/3 trailing

 

 

as far a forcing all axis output in plinout....

 

if not(cuttype <> 0 & xinc = 0 & yinc = 0 & zinc = 0 & ainc = 0 & cinc = 0), #avoid output of feed with no motion when changing between G93 and G94/G95

[

if mill5$ = 1 & lock_codes = 1, #Force output to avoid axis locking when the lock_codes aren't being used

[

pcan1, pbld, n$, sgfeed, sgplane, `sgcode, sgabsinc, pccdia,

pfxout, pfyout, pfzout, pfaout, pfcout, `feed, strcantext, scoolant, e$

]

else,

[

pcan1, pbld, n$, sgfeed, sgplane, `sgcode, sgabsinc, pccdia,

pxout, pyout, pzout, paout, pcout, `feed, strcantext, scoolant, e$

]

if cur_cflg$ = 70000,

[

#pbld, "M00", e$

#pbld, "(TOOL INSPECTION POINT)", e$

ptlchg$

]

]

 

The two attached images are how my machine and control def are set.

 

HTH

[Rotary Ninja]

Wow.

[The_kid]

wow indeed does some really impressive stuff.

[Bob W.]

Jeremy, those settings have Mastercam puking all over the place (corrupted files, strange post issues, etc...). For whatever reason the tight tolerances are making a mess of things, and this is for my three and four axis machine definitions that had been working great before. I do have the 5th decimal place working though. Thanks for the help.

 

Bob

[gcode]

Jeremy, those settings have Mastercam puking all over the place (corrupted files, strange post issues, etc...). For whatever reason the tight tolerances are making a mess of things, and this is for my three and four axis machine definitions that had been working great before. I do have the 5th decimal place working though. Thanks for the help.

 

Bob

 

I'm assuming you are running X6

Do you keep your control defs in your user folder.. or somewhere else

If they are somewhere else, look in that folder.. and look for goofy filenames.tmp

If you've got them, contact your dealer and request the X6 control def fix.

[Bob W.]

I am still running X5 and I keep my control definitions on a server.

[GnoGueyJose]

X5.... Ewwwwwwwwwwwwwwwwwwww!

[Bob W.]

X5 with Volumill, definitely not Ewwwww! With the work I do there aren't enough improvements in X6 to offset what I would be losing by not having Volumill available. The main thing is 100% efficient rest roughing on very complex geometry, but that is another thread... I can install X6 any time I wish but I choose not to.

 

http://www.emasterca...showtopic=71828

 

Didn't want to hijack this thread. but I have ZERO of these issues with Volumill. First try, every time and it takes 5 minutes.

[Jeremy Herron@DBS Solutions™]

Shoot me a .z2g so I can help you diagnose your problems.

[Bob W.]

Shoot me a .z2g so I can help you diagnose your problems.

 

Will do. I'll try to get it to you in the next day or two. Thanks for the help!