[squarewave]

Does anyone know offhand if helical interpolation is supported in V14.2 Pro? When I include a Z value in the G2/G3 with an I and J, I appear to get a circle in either the XZ or YZ plane. I've tried it with G17 and without.

I see a supplied macro that appears to approximate this function using the POLAR command, but I just wanted to make sure I wasn't missing something.

I also looked through the Galil manual in hopes of using a direct command but I don't see a simple solution there either. There is mention of potentially using a slave and gearing but no example.

Thanks!

[Karl_T]

It is supported but I remember the control doing funky thing too. Try starting at 0,0,0

G0 X0 Y0 Z0
G0 X1
G2 X1 Y0 I0 J0 Z-.1 '(FANUCARC absolute)

Control should make a helical arc

[Lohmeyer]

It is probably related to your tolerance setting. If TOLERANCE is too tight relative to the Z component of the arc move, G02/G03 commands with a z component can be misinterpreted and result in an arc in the wrong plane! It's been a while since I looked at this issue so I forget exactly what the interactions are. I think I had this issue when I was playing with TOLERANCE = 0.0001, but it went away with TOLERANCE = 0.001, for example. I think it was small Z values with a small TOLERANCE that did it. Large Z values didn't cause it. It may have also been influenced by my ARCFACTOR value. A large ARCFACTOR may have made it worse (??).

Also, in CNCSetup, under the Motion Settings tab, make sure "Do not keep track of fractional counts" is _unchecked_. This is very important. If it is checked, then helical arc moves (arc moves with a Z component like helixing down into a pocket) will have Z errors that can accumulate and result in severe error, or cause the machine to stall out due to an over tolerance condition. When checked, rounding errors or fractional counts are kept and added together, resulting in the commanded Z and the actual Z movement not being the same. E.g. after helixing down into a hole to say Z-5.0 (in mm), the actual stopping point I would see would be in error by as much as 0.5mm. Meaning it would stop at -5.5mm.

I don't remember if this affected the problem of an arc move changing planes, but while I was trying to solve this Z depth issue, I had lots of cases where an XY plane arc changed to XZ or YZ like you describe.

Regards,
Mike

[squarewave]

Karl,

Thanks for the reply. I've tried your program with Z values ranging from .01 to 1. I keep getting vertical circles. I have FANUCARC 0, which is absolute.


Mike,

Very interesting. My TOLERANCE setting is .001 and my ARCFACTOR is 100. I have yet to get a helix in the XY plane regardless of the Z value I use. I do not have "keep track of fractional counts" in my Motion tab, just Ratio, Gear, and Tool/Degree.


So both of you have seen this behavior, though it sounds like mine is more consistant - especially since I have yet to see a helix.

The macro that I referred to that was supplied by Camsoft uses short vectored moves in the XY plane using the POLAR command, then plunges Z a small amount after the POLAR move is complete. This is done in a loop until the 'helix' is complete. I don't know why this macro would have been provided if V14.2 supported helix moves in G2/G3 moves.

Thanks for the replies. Looks like I'll have to write a macro that does this with linear moves.

Scott

[Karl_T]

If you are comfortable with Galil commands, this would be a very simple program there. The only requirement that might get you is your X and Y must have the same counts per inch or you get elipses. I'm just about positive if you download the 1800 manual from galilmc.com there is an example of this to copy and paste.

Karl

[Karl_T]

http://www.galilmc.com/support/appno...a/note2426.pdf

if you want to go galil comands

[squarewave]

This looks GREAT Karl, thank for posting it. I'll see if I can get something going.

Scott

[Karl_T]

Say, I was on the road when you first asked. I just read the manual (normally a good first step)
Looks like you need to specify both K and Z to get a helical motion

Try starting at 0,0,0 with a K value

G0 X0 Y0 Z0
G0 X1
G2 X1 Y0 I0 J0 K0 Z-.1 '(FANUCARC absolute)

Control should make a helical arc

CCW
Turns a counterclockwise arc. An active feed rate MUST be in effect prior to issuing this command. Failure to do so will cause the machine tool control program to simply not move and appear to be “hung up.” You may use the ESC key to cancel the movement if this should occur. A true spiral helix or helical arc can be easily made. If the Z axis value specified differs from the K or Z axis arc center, then the arc will create a helical motion from the start of the arc to the end. There are 5 extra optional parameters to be used only if needed for axes 4 through 8 for positioning while turning the arc. The 4th through 8th axes positions can be optionally specified directly after the last parameter in order starting with the 4th axis. Skip any parameter by issuing only a semicolon. If these parameters are not given, the current positions of these axes are used. If the parameter is skipped, then the last axis letter issued is used. If a value is given, then this axis will be forced to the position issued in a coordinated motion with the arc.
EXAMPLE: CCW x;y;z;i;j;k
CCW x;y;z;r
CCW x;y;z;i;j;k;a;b;c;u;v
CCW x;y;z;r;a;b;c;u;v

[squarewave]

Karl,

Thanks for posting that information. What version is that manual for? My v14 manual mentions nothing about helical, and none of what you suggested gives me a helix on my machine. Typically, the K value will be the pitch when the Z values are different in a G17 plane. I feel like I've tried all of the combinations typical on other controllers. I believe helical is just not supported in G2/G3 in V14.2.

I feel like I've about got the problem licked with the Galil gearing, EXCEPT, I can't seem to get out of the Galil program gracefully. When I complete the helix, I cancel the mode and the gearing. I then have a Z rapid to return to the rapid plane. The program just stops at that command and hangs (never executes the command). Here is most of the program:

RAPID {x+\500};y
WAITUNTIL STOP2:WAITUNTIL STOP1
RAPID ;;\510
WAITUNTIL STOP3
SLEEP .5
COMMAND ST
COMMAND VM XY 'XY Plane
COMMAND VA 50000 'vector acceleration
COMMAND VD 50000 'vector deceleration
COMMAND VS \503 'vector speed
COMMAND GA ,,S 'vector motion as master for slave Z
COMMAND GR ,,-\505 'define Z axis gear ratio
COMMAND CR \501,0,\502 '\501=radius in counts 0=start angle \502=end angle
COMMAND VE 'vector end
COMMAND BGS 'begin sequence
WAITUNTIL STOP2:WAITUNTIL STOP1:WAITUNTIL STOP3
SLEEP .5
COMMAND GR0 'cancel gearing
COMMAND LM XYZW 'return to linear axes
SLEEP 2
RAPID ;;\510 'move to rapid plane
FEEDRATE \509
WAITUNTIL STOP3

The RAPID after SLEEP 2 never executes and does not generate an error. I've also run it in DIAGNOSTIC mode and there are no clues there either. The rest of the program executes perfectly.

Does anyone have any suggestions?

[Karl_T]

V14 is pretty old. I'm current with V17.


I use a different approach. Get your Galil programs working without Camsoft running. Put them all in a .DMC file and load them at startup. Here's one program for homing:



DOWNLOAD C!/AS3000/CNC/JOGnHOME.DMC 'load jogbuttons and homeall into Galil card
(Note version 14 had another way to do this)


Run the program like this:
COMMAND XQ #AXIS3HM 'execute Galil home routine



Here's my axis homing program.
'Below homes 3 axis simultaneously, X axis reversed to home
'done varible used in Camsoft to test for macro complete
#AXIS3HM
done=0
CN,-1
SP 0
MO
CE 2
MT -1
SH
SP 5000,5000,5000
HM
BG ABC
MC
SP 0,0,0
MO
CE 0
MT 1
SH
done=3
EN

[squarewave]

I saw examples of downloading programs to the card, but I didn't see how to pass variables to the program - like radius and pitch. Do you have any experience with that?

[Karl_T]

I think its just:
COMMAND var=1
to set var to a value of 1


here's an example to put Camsoft in a hold loop

COMMAND HX 'Halt Jog buttons
COMMAND XQ #AXIS3HM 'execute Galil home routine
:HOMINGLOOP
SLEEP 1.0
COMMAND done=?: RESPONSE \55:IF \55<3 THEN GOTO :HOMINGLOOP 'done is variable in Galil program
\138=0 'allow JOG to load