Haas Guru Needed

[Jim at Gentex]

Good day all.

 

I am new to running our Haas VF4 w/ AB trunion table and ran into problems with cutter comp.

Is there a parameter to turn on / off 2D and 3D cutter comp?

If so, does anyone know what they are?

 

It seems to me like it's something that simple...

[Matateu]

Hi,

What is the error that gives the controller?

[Jim at Gentex]

Incorrect I,J, or K value.

 

But the syntax looks right.

 

(T7 - 3/8 FLAT ENDMILL - H7 - D7 - D0.3750" )

N100 G00 G17 G20 G40 G49 G80 G90

N101 (TOOLPLANE NAME - TOP)

N102 G90 G54 X0. Y0. ( TOOLCHANGE POSITION )

N103 T7 M06 ( 3/8 FLAT ENDMILL)

N104 M01

N105 (MAX - Z2.)

N106 (MIN - Z0.)

N107 M11 (B-AXIS UNLOCK)

N108 M13 (A-AXIS UNLOCK)

N109 G00 G17 G90 G54 A0. B0.

N110 M10 (B-AXIS LOCK)

N111 M12 (A-AXIS LOCK)

N112 G00 X-5.55 Y0. S2500 M03

N113 G43 H7 Z2. M08

N114 G94 Z.1

N115 G01 Z0. F5.

N116 G42 D7 X-5.55 I.25 J0.

N117 G02 X-6.05 I-.25 J0. F10.

[Matateu]

This has to do with the fillet and the plans that you are using, you are using the G17?

can put the line of code where the error?

[Matateu]

In the offset table place the D7 to 0 and see if it continues to give the same error.

[Matateu]

I think we also can not put the G42 along with the G02 and G03 only with G01

 

[Matateu]

N115 G01 Z0. F5.

N116 G42 X-D7 5:55 J0 I.25.

 

I and J = G02 and G03 not G01

 

I think this is incorrect. must turn in your mastercam inputs and outputs of the tool, for at least 25% of the tool diameter in radius and line so you can compensate for G01 not to give error.

[htm01]

I don't think haas can enter CC on an arc, must be line

[Guest MTB Technical Services]

Jim,

 

Your code is incorrect as it's attempting to engage CRC in a modal G01 move with the I & J components for a non-existent arc.

 

Modify your lead-in/lead lead//out settings so you aren't so close to the max length for

the linear move required to engage CRC.

 

 

CRC requires a linear move to engage it on Haas and Fanuc.

Always engage CRC with a perpendicular linear move and then a ramp move into the part.

This method will allow you to engage CRC and minimize witness lines at the engagement of the part.

[Machineguy]

MTB is correct. The logic is off in line N116. CC MUST to start on a G1 line to work or Hass will give you a error. Add a lead in and lead out to that section of the file and repost. It should give you a G1 and G42 together. The next line will have a G2 or G3 lead in.

In any case the post logic is not correct. G42 should not have kicked in without a lead in and then a arc. Just to let you know, Haas will run with a .0001 lead in and a .0001 arc for CC. I haven't tried it on the newer control software but it does work on the older ones.

 

Machine guy

[Jim at Gentex]

Thanks much for the input all.

 

I'm totally new to this control so your info is very helpful.

 

I have a different job running at the moment, but I will get back to the Haas shortly.

I will post an update when I get back to it.

 

Thanks again.

[Jim at Gentex]

OK I've found that I can't even mill a simple circle without cutter comp!

 

I am entering:

 

G00 X-5.8 Y0 (initial position)

Z-0.1 (1st depth cut)

G01 Y1. F5. (linear move to top of circle)

G90 G3 X-5.8 Y1. I0 J-1. (mill circle)

Y0 (linear move back to center)

 

I get error: "Invalid I, J, or K in G02 or G03"

 

Are you guys saying the G01 linear move needs to be on the same line as the G03?

[Guest MTB Technical Services]

OK I've found that I can't even mill a simple circle without cutter comp!

 

I am entering:

 

G00 X-5.8 Y0 (initial position)

Z-0.1 (1st depth cut)

G01 Y1. F5. (linear move to top of circle)

G90 G3 X-5.8 Y1. I0 J-1. (mill circle)

Y0 (linear move back to center)

 

I get error: "Invalid I, J, or K in G02 or G03"

 

Are you guys saying the G01 linear move needs to be on the same line as the G03?

 

 

You are trying to move back to Y0 in a linear move without coding a G01.

G02/G03 are modal.

You are getting the error because you have specified an endpoint for an arc without all the required data.

Anytime you change from linear to arc or arc to linear the appropriate interpolation code must be included.

In this case, you need a G01 on the Y0 move back to center.

 

Try entering this code manually

G00 G90 X-5.8 Y0 (initial position)

Z-0.1 (1st depth cut)

G01 Y1. F5. (linear move to top of circle)

G03 J-1. (mill circle)

G01Y0 (linear move back to center)

[Guyinthedesert]

OK I've found that I can't even mill a simple circle without cutter comp!

 

I am entering:

 

G00 X-5.8 Y0 (initial position)

Z-0.1 (1st depth cut)

G01 Y1. F5. (linear move to top of circle)

G90 G3 X-5.8 Y1. I0 J-1. (mill circle)

Y0 (linear move back to center)

 

I get error: "Invalid I, J, or K in G02 or G03"

 

Are you guys saying the G01 linear move needs to be on the same line as the G03?

You need a G1 on the last line, Y0

[GIZMO 21]

Naa jim the cutter comp start should be on a g1 move.if your doing a straight cut.set it in your

Lead in /out parameter page.if your using it in circle mill adjust in your start/end angle parameter page.

[GIZMO 21]

I also try to cancel cutter comp with a g1 move setting the same parameters.

[Jim at Gentex]

OK thanks all.

I'm at the point now where I'm not even using Mastercam.

I just want to get the thing to mill a circle first so I can see what the correct syntax looks like!

 

I see Tim's explanation and I think I get it now.

Man...it's just been that kind of day.

 

[crazy^millman]

OK thanks all.

I'm at the point now where I'm not even using Mastercam.

I just want to get the thing to mill a circle first so I can see what the correct syntax looks like!

 

I see Tim's explanation and I think I get it now.

Man...it's just been that kind of day.

 

 

So you need to come to a Mastercam Forum to get help on another CAM Software is what you are saying?? J/K hope all is going well.

[htm01]

try out the quick code on the machine, if you have the option, good for circles and pockets.

[Jim at Gentex]

OK well I followed the format Tim gave me and it works.

 

I still can't understand why the help menu gives the syntax : G03 X? Y? I? J? but it doesn't work.

 

Anyway I'm a little less confused now, and at least I can mill a circle!

I added my G42 line for cutter comp and everything seems to be working as it should.

I will need to look into my post later to get it to output the correct syntax, then I should be good to go.

 

Thanks again all for your help.

[Guest MTB Technical Services]

OK well I followed the format Tim gave me and it works.

 

I still can't understand why the help menu gives the syntax : G03 X? Y? I? J? but it doesn't work.

 

Anyway I'm a little less confused now, and at least I can mill a circle!

I added my G42 line for cutter comp and everything seems to be working as it should.

I will need to look into my post later to get it to output the correct syntax, then I should be good to go.

 

Thanks again all for your help.

 

The help menu is correct.

You didn't add the G01 for the linear move back to Y0.

That's what generated the error.

The control was still in G03 mode but only had a Y0 on the line.

[Jim at Gentex]

Aaahh yes...I see.

Thanks again, Tim.

 

I'm trying to do two jobs at once this afternoon and not doing very well on either one!

I've been working exclusively with a Heidenhain control for quite a few years, so this Haas control is all new for me.

Once I get the post dialed in for correct circle milling I should be good to go.

 

Once again the eMC forum comes through!

[Matateu]

Hi Jim,

 

In HAAS machines there a tool that will help you make small programs. Tool is called Visual Quick Code. See if you have that extra in your machine.

 

http://www.haascnc.com/sappi/documents/options/IMAGE_VQCZWD00001.jpg