Rotary unwinding

[mmoya]

We have a new VF-4 with the HRT-210 rotary, we're using the rotary for the first time on this machine and so I wrote some test programs to make sure everything moved correctly.

My tester was a spiral shaped contour along X and I used axis substitution for Y so the spindle basically just sits at Z and moves along X while spinning the rotary, now after 10 or so revolutions the rotary winds up to about 4000 degrees, and when the spindle retracts for a second pass & commands A0, the rotary has to unwind all the way back to 0 which is suuuuuper slow.

G91 G28 A0 fixes the problem but I have to punch it in manually between passes. I tried browsing through the post to see if I could find something for it to no avail.

I went into the MD on mcam and selected "Shortest direction, absolute angle" instead of "Signed continuous" and that didn't change anything either.

Could someone help me out?

[Colin Gilchrist]

If you look inside the post, there is a "switch" variable: 'frc_cinit'. This stands for "force C initialize". This will cause the post to output "A/B" or "A/C" zero. You can modify that post block to output the Incremental return for the rotaries. It will be a simple post edit. In order to make sure it resets between toolpaths, you might need to use "Force Tool Change" on the next operation, to make it force a return to zero...

[mmoya]

I searched that variable and it comes up three times.

Once in the Rotary Axis Settings section:

frc_cinit    : yes$

Once in the Start of File and Toolchange Setup section, about 40 lines down from "pretract #End of tool path, toolchange"

 #cc_pos is reset in the toolchange here
      cc_pos$ = zero
      gcode$ = zero
      if use_rot_lock & rot_on_x,
        [
        if (index = one & (prv_indx_out <> fmtrnd(indx_out)) | (prv_cabs <> fmtrnd(cabs)))
          | nextop$ = 1003 | frc_cinit, prot_unlock
        ]

And once more in the same section but further down,

protretinc      #Reset the C axis revolution counter
      if frc_cinit & rot_on_x,
        [
        rev = zero
        sav_rev = zero
        cabs = zero
        csav = zero
        indx_out = zero
        if index, e$, pindxcalc, pindex
        else, *cabs
        prvcabs = zero
        !csav, !cabs
        ]

rot_on_x is turned on, and use_rot_lock is off.

 

I'm not sure what i'm supposed to change..

I'd rather not have to force a toolchange because then it puts an M01 after each pass. I put M01's in the program sometimes in case i need to tell the operator to do something, and if op-stop is on, then it retracts and stops all the time which defeats the purpose of it...

[mmoya]

bump

[Brian Pallas]

The Haas might have a setting to just go back to the zero point instead of unwinding. I've never used it but I think I remember seeing something like that. Maybe ask a Haas Apps guy and you can go on their site and ask the Answer Man.

 

 

Sent from my iPhone using Tapatalk

[MIL-TFP-41]

What post are you using?

 

Also you can set your rotary limits in your machine def to what is on the attached screenshot. I use MPMASTER and it does not "wind up" with the these settings.

 

 

[Brian Pallas]

http://int.haascnc.com/magazine_article.asp?intLanguageCode=1033&VolumeNo=-1&IssueNo=11033&ArticleID=1459

[mmoya]

What post are you using?

 

Also you can set your rotary limits in your machine def to what is on the attached screenshot. I use MPMASTER and it does not "wind up" with the these settings.

I'm using the included "Generic HAAS 4X Mill." If I set my min/max to those values, what will happen if I post a axis-sub toolpath like the one that commands 4k degrees?

I've been reluctant to switch to MPMASTER because I don't know how the machine will behave. I'm having a hard time understanding the post and how to modify it without fcking anything up.

 

Here's a snip of my program for reference, you can see where I had to manually add the G91 G28 A0 & G90.

N66460 G94 G1 Z1.0067 F5.
N66470 G42 D2 X-.4429 A-298.034
N66480 X-.4061 A-297.959
N66490 X-.3696 A-297.606
N66500 X-.3337 A-296.981
N66510 X-.2988 A-296.091
N66520 X-.2652 A-294.943
N66530 X-.2332 A-293.549
N66540 X-.2032 A-291.922
N66550 X-.1754 A-290.079
N66560 X-.1501 A-288.036
N66570 X-.1275 A-285.814
N66580 X-.108 A-283.433
N66590 X-.0915 A-280.917
N66600 X-.0784 A-278.29
N66610 X-.0687 A-275.578
N66620 X-.0625 A-272.806
N66630 X-.06 A-270.
N66640 G93 X1.14 A4050. F.1
N66650 G40 A4410. F.8
N66660 G0 Z1.2567
N66670 X-.8178
G91 G28 A0.
N66680 G90 Z1.2067
N66690 G94 G1 Z.76 F5.
N66700 G42 D2 X-.4429 A-298.034

http://int.haascnc.com/magazine_article.asp?intLanguageCode=1033&VolumeNo=-1&IssueNo=11033&ArticleID=1459

I've done this already, hence why I explained that manually typing in G91 G28 A0 works in my op.