A G43.1 Question

[robk]

True... This is on our Mazak

[crazy^millman]

We do the same thing on the Integrex Rob. I use G43.4 all the time or G68. I do all my lathe programming normal then my milling porgrams as those 2 and never have a problem. We just finish this trick fixture I designed and programmed all in EIA no problems.

 

G I do all of the Integrex programming with the G43.4 in inverse time and have not have a problem. Like mentioned before just need the G49. The Integrex needs the G49 after retracts move where the C axis is going to move a real pain, but if you don't there is a crash. I hope your machine handles switching from G43.4 to G68 better than our Integrex we have to reset the machine anytime this happens and since the control is considered old by Mazak they have pretty much told us tough S??T. The GENERIC 5 axis post will handle all of this if you need some help tweaking you got my number.

[bob161]

We have a new 5 axis router with a Fanuc 18i M PC based control, and are in the process of sorting out the post and getting the hang of G43.4.

 

Previously we have always programmed by telling the post the tool length and pivot point, then letting the post do the maths. But now we want to use G43.4.

 

 

At the moment to get it roughly working the way I think it should-

 

 

I have to add the tool length of 204mm (tool tip to spindle face) and the pivot distance of 170mm (pivot point of the B & C axis to the spindle face) and enter the total in the tool offset table i.e. 374mm. This make the tool tip behave correctly, but the toolpath starts 170mm to high.

 

If I only enter the tool length, the toolpath starts at the right height, but the tooltip is all over the place.

 

 

So I'm guessing there must be a parameter for the pivot distance that has not been configured on our machine?

 

 

Also I've got it coming on OK, but having trouble turning it off.

 

We normally finish our programs with

 

G05 P0

G91 G28 Z0.

G91 G28 X0. Y0. B0. C0.

G90 G49 G40 G80

M30

 

But this alarms out on the G91 G28 Z0 line.

 

 

If I add a G49

 

G05 P0

G49

G91 G28 Z0.

G91 G28 X0. Y0. B0. C0.

G90 G49 G40 G80

M30

 

I works OK, but the tool comes down in Z by the tool offset value on the G49 line. How do you get around this?

 

 

And just to double check. G43.4 takes care of the feed rates also, so no need for inverse time feed? And can you use it for normal 2.5D and 3D surfacing paths?

 

 

Thanks for your help.

[robk]

Bob161 Welcome to the forum.

 

You should not be adding the pivot point distance value into your TLO. Check your parameter manual for info. You probably should have 2 parameters related to the pivot point. One is for the distance from the rotational center of the B axis to the tool center, and the 2nd is the distance from rotational center of the B axis to the spindle edge. (On Mazak they're BA61 & BA62)

 

You should also have a parameter to cancel your TLO without the axis movement (On Mazak it's F114 Bit 1).

 

And yes... You do not need to use inverse feed rate when using G43.4

[crazy^millman]

quote:

---

I works OK, but the tool comes down in Z by the tool offset value on the G49 line. How do you get around this?

---

I would change my post so that if I used G43.4 it would call up G49 before with a safe move of say Z6.0 or something of that nature. I did this on a Thermwood router years ago when calling G49 and it would keep it from moving down to violate the part.

 

HTH

[bob161]

Thanks guys.

 

I've found the parameters for the pivot point. But not found one yet for G49. I'd rather it didn't move, just in case my tool is longer than the safe move Or the safe move is longer than the travel left.

 

I'll take the Fanuc manual home for some light reading, or give them a ring.

 

Cheers.

[gcode]

bob1.. I went thru the same thing with a new 5axis machine and G43.3 on a Fanuc 15m.

The rapid move when G49 is applied cannot be

prevented..

from the manual

TOOL BEHAVIOR AT START AND CANCELLATION

 

When tool center point control is started (G43.4) or canceled (G49), the tool moves by a tool offset value.

 

Compensation vector calculation is performed only at the end of the block.

 

I guess G43.1 is the same

[john316]

.

 

bob161,

 

Look in the "pretract" section of your post and add this line:

 

pbld, n$, sgcode, "G90", "G53", "H0", "Z0.", e$

 

before this line:

 

pbld, n$, *sgabsinc, *sg28, "Z0.", e$

 

The G53 is a machine return command and will make your z-axis return to machine zero instead of trying to drive through the table.

 

HTH

 

.

[gcode]

This worked for me, but if the machine does not see G49 in the next line it overtravels in Z

When it reads the G49, it rapids straight down

the distance of the length offset.

At least its doing it from Z home so its normally a safe move.

I had 3 different Fanuc experts look at it and

they were unable to prevent this behavior.

[bob161]

quote:

---

I guess G43.1 is the same

---

I used to program using G43.1 on a Mazak with Fanuc control, and that allowed G91 G28 Z0 followed by a G49 without the operator panicking Z dive.

 

I've just dug this up at home -

 

G00 G17 G21 G40 G49 G80 G90

G91 G30 Y0. Z0. A0. B0.

T1

M6

G90 G00 A0. B0.

S1000 M03

G00 G90 X339.0 Y-141.5 A0.0 B0.0 M03

G43.1 H1 X339.0 Y-141.5 Z41.9 A-17.0 B0.0 M08

{

{

G01 X-314.0 Y-154.664 Z-1.066

G00 X-314.0 Y-141.507 Z41.968

G40 M09

G00 G90 A0.0 B0.0

G00 G91 G28 Z0.0 M5

G49 Y0.0

M01

M99

 

Maybe it's a Mazak thing, or the two codes allow different commands.

 

I'll have another play tomorrow.

 

If I can get the machine to the Z & X home position using G53, as long as no one is stood under the tool, then the Z dive should be OK .

 

Thanks Again.

[MLS]

Our solution to this was to capture the last z output and add the maximum tool length we use (8 inches) prior to outputting the G49 and let the post calculate this at the end of every tool.

 

.

.

.

X34.5 Y23.1

G00 Z2.83

G00 Z10.83 (LAST Z(2.83) + 8) ADDED LINE

G49

G00 G91 G28 Z0

T2 M06

.

.

.

[Mic]

If you change parameter 5006 #6 ( bit 6 ) from 0 -> 1 the control should cancel G49 without any movement.

[bob161]

quote:

---

If you change parameter 5006 #6 ( bit 6 ) from 0 -> 1 the control should cancel G49 without any movement.

---

Cheers. Not had chance to try it yet. They gave me some real work to do.