A G43.1 Question

[gcode]

All my 5X experience has been gage length programming... you tell Mastercam how long the tool is and the post outputs tooltip numbers

and tooltip feedrates.

We are getting a machine with the G43.1 and I'm not sure what I want to post.

It seems to me that you'd want to output the

actual part numbers for gcode and the feedrates

at the pivot point.

Then the machine can compute both the length offset and adjust the feedrate to the actual length of the tool.

 

Edit ... the control is a Fanuc 15i-M

 

[ 09-05-2007, 02:28 PM: Message edited by: gcode ]

[gcode]

quote:

---

What does the control's operating and programming manual list for the G43.1?

---

You don't think they would actually give me an operators manual do you

 

The dealer is still building the machine and has not turned control of it over to us yet. I'll have to run over there and see if I can "steal" a copy of the maunal.

 

edit... Well that didn't work... the machine builders don't speak English and I don't speak Chinese.

Here is a picture of the machine

[MLS]

Mazaks w/ Fanucs that we use G43.1 for are set up as follows:

 

Post compensates Position/FR for pivot distance.

Machine compensates for Tool length offset.

 

 

Does the new(I assume) machine have a G43.4 option?

 

Edit:

Ahhh. A Viper. I used to run one of those.

[crazy^millman]

Tom where were switching the SNK gantry over at the place we worked after you left and before left. The machine would take the given gauge length and adjust it to a known gauge length. Best set-up with this is where you have a tool eye and the machine does all the work for you, but doubt that one comes with one. Shoot Kevin and email he got into it pretty good on that machine he is still involved with from what I remember.

 

HTH

[gcode]

quote:

---

Does the new(I assume) machine have a G43.4 option?

---

I'm guessing it does.. the machine is new and the control is supposed to be loaded

 

I know it has G68 3d coordinate rotation

 

Every 5X machine I've ever run had a totaly stripped control so this is all new to me.

 

I've alwasys programmed gage length and feedrate

to the comped tool tip.

 

[ 09-05-2007, 03:33 PM: Message edited by: gcode ]

[MLS]

Realize this is based on the machines I am familiar with. Mazak Vortex with a 31i Fanuc and Makino Mag series with Proffesional 3 & 5(Fanuc based). There may be some differences.

 

 

If it does have a G43.4 option then that is the best case scenario IMO. G43.4 allows you to program tip of tool totally. The post would output exactly what comes out of Mastercam and the control compensates for pivot distance and tool length. Some controls even have options to compensate for feedrate so you can output linear instead of inverse time.

 

 

If it only has a G43.1 option(2nd Best IMO) then the Post should be set up with the pivot distance of the machine and inverse time feedrate, but the individual tool offsets should all be set at the machine. This eliminates the need to set the tools to a specific gage length as the tool length offsets are all in the control and compensated for.

[Plastmo]

G43.1 or G43.4 is full 5 axis dinamic

cutter lengh compensation. For 3D programming

You gonna use G43 as normal.

You've got to enter tool gauge to tool register

and thats all.

Do not forget to change pivot point lengh in

Your post to 0. valu, becouse You are programming tool tip.

[gcode]

Thanks.. that makes sense.. now I just have to find out what options the control actually has.

Either G43.1 or G43.4 is a big improvement

over gage length programming.

The salesman is suppossed to be by sometime today.

I guess I'll have to sit him down and make him define "loaded"

[sharles]

We just got the 43.4 option added to our Fanuc control. I haven't had to change how I do my mastercam programs (maybe I should have and we didn't know better), but the 43.4 is supposed to do away with some of the nasty shortcomings of 43.1. So far the operators have been fairly pleased with it. Definitely look into that option.

[DavidB]

This might be a silly question guys. Is G43.1 and G43.4 used only on 5-axis machines where the tool does the 5-axis moves or would you still use these codes for a 5-axis machine that the spindle is fixed (moves in XYZ only) and the rotations are done by a rotary rotary table?

[Bruce Caulley]

David,

It is a different animal if it as a table table. In a head/head the thing that has the most effect on tool position is the length, hence the G43.1 On a table/table the critical factor is workpiece position. That is why table/table machines with dynamic comp use G54.1

 

Gcode,

I was programming for a Mazak Vortex and the post was setup to use G43.1

 

Here's the rub. The control compensates the position of the tool as it knows the pivot distance and the tool length. For the feedrates, assuming your post is setup for inverse feed, you will need to enter the pivot distance in the post and have a correct tool length in your tool definition. Note that if you have the tool length and pivot distance wrong in the post/MC file that the feedrate will not be correct. At the same time there is no need to go overboard with decimal places.

 

HTH

 

Bruce

[gcode]

quote:

---

For the feedrates, assuming your post is setup for inverse feed, you will need to enter the pivot distance in the post and have a correct tool length in your tool definition.

---

Meaning G43.1 comps only the tool and not the feed rate. The value entered in OAL of the tool's parameter page must be resonably close to get accurate feedrates.????

[gcode]

quote:

---

but the 43.4 is supposed to do away with some of the nasty shortcomings of 43.1.

---

sharles.. can you elaborate??

 

gcode teh attentantive student at 5X comp school

[robk]

Using G43.4 you don't have to worry about inverse feed rate.

[gcode]

OK.. the machine is going to have G43.4

Since I don't have a manual yet I don't know

what I need for post output

I assume I want the post to output the gcode

with no comp at all and feedrate should be linear.

 

My question is when do I use the G43.4

Do I use G43 for regular 3X toolpaths and G43.4

for everything else, or just use G43.4 all the time??

[robk]

This is on my Mazak.

Use G43.4 only when you need to. When you lift the tool and go to another place on the part it will take the closest route (could be right through the part). One way to omit that is to cancel the TLO with a G49.

When using wear comp with the G43.4 your G41's will have to be changed to G41.5.

Your drill canned cycles will not work with G43.4. I use point-to-point or G68 when I feel like it...

If you're interested I could send you a couple of pdf's regarding Mazak programming using tool tip comp.

[gcode]

Rob.. you've got mail

[robk]

Here is a little sample of code...

 

 

quote:

---

()

()

N20 T26 M06 T25

G65 P9862 B3. T26 D26 I.250 /2S3000 (SET TLO AND WEAR)

()

()

( Tool Name : T26_.250_ENDMILL Tool Diameter: 0.250)

()

()

G20 G69 G80 G40 G49 G17 G90 G94

G10.9 X0. (SET RAD MODE)

G91 G28 Z0.

G28 X0. Y0.

( Path Name : BLEND RADII)

M200 (C AXIS CONNECTION)

M108 M212 ( B AXIS UNCLAMP C AXIS UNCLAMP)

G55 G00 G90 B96.776 C92.009

S15279 M03

G00 G43.4 H26 X15.3789 Y-.9742 Z3.249 B90. C357.48

G61.1 M08 (HIGH ACCURACY MODE)

G01 G41.5 X15.3711 Y-.9966 Z3.2411 F45.8 D26

X15.3776 Y-.9977 Z3.2381

X15.3822 Y-.9989 Z3.2353

X15.394 Y-1.0036 Z3.225

X15.4012 Y-1.0083 Z3.2152

X15.4093 Y-1.0177 Z3.1964

X15.4122 Y-1.027 Z3.1782

X15.4052 Y-1.0774 Z3.1381 B96.743 C92.12

X15.37 Y-1.4396 Z3.0962 B96.185 C93.425

X15.3486 Y-1.5842 Z3.0545 B95.875 C93.935

X15.3257 Y-1.7364 Z3.013 B95.462 C94.49

X15.3026 Y-1.8813 Z2.9717 B94.964 C95.035

X15.2824 Y-1.9971 Z2.929 B94.46 C95.487

X15.2663 Y-2.0812 Z2.8867 B93.995 C95.834

X15.255 Y-2.1366 Z2.8451 B93.602 C96.084

X15.2252 Y-2.2861 Z2.7908 B92.075 C96.757

X15.2211 Y-2.2636 Z2.737 B91.975 C96.786

.

.

.

.

.

.

.

G00 X18.57

Z15. M09

G64 M05 (CANCEL HIGH ACCURACY MODE)

G49 (CANCEL TLO)

G91 G28 X0. Y0. Z0. B0. C0.

M850 T26 S3000 W.005 (TOOL BREAKAGE DETECTION)

M01

()

.

.

.

.

---

[sharles]

quote:

---

sharles.. can you elaborate??

---

Gcode, I'm no expert, but with G43.1 the feedrate can vary to the extreme. In fact I just had one 5 axis part that kept snapping endmills and I think it had to do with how it calculated it's feedrates. I programmed it for 30ipm but only one axis had to move at a certain spot and it ramped up to 180ipm. That doesn't seem to happen any more with the g43.4. Probably the inverse feedrate everyone keeps mentioning. Also with g43.1 the tool does NOT really move at the tip of the tool (all the time) meaning retract/rewinds can do some very violent dancing of the the b and c axis (so we just had to move it up real far in Z to keep it away from the part). Now the operators tell me with g43.4 that seems to have significantly gotten better.

 

I haven't really been out on the machines to see the g43.4 in action, but as I said our operators are much happier with it.

[john316]

.

 

Sounds like you have most of your answers G. I haven't used the G43.4, but with either G43.1 or G43.4 the machine should calculate the inverse feed based on your input. If it does it will calculate based on the pivot distance and tool gauge length. With the G43.1 you put the pivot distance in the post, G43.4 the machine does it all.

 

I would try both linear and inverse in your post to see what difference it makes in your machine response.

 

With the G43.1 I use it even for 3d work so I don't have to have 2 posts or set-up variables base on the type on opcode I'm using.

 

BTW, If you think it's hard talking to that machine supplier, wait until you try and read the manual, lol.

 

.

[robk]

One more piece of info you might be interested in is that you can't use G02/G03 when using G43.4. Need to break the arcs into lines.

BTW, did you get the attachments gcode?

[gcode]

Thanks for all the info guys.. I've got enough

to get started..

I've got a good working post and can try

both methods with minor hand editing.

It would probably be best to do some experimeinting before finalizing the post requirements.

Rob, I did not recieve the pdf's, or an email.

Probably an over zelous spam blocker on one end ot the other. I'll send you an alternate email

address

[gcode]

quote:

---

BTW, If you think it's hard talking to that machine supplier, wait until you try and read the manual, lol.

---

I got the same answer to every question..

"So sorry sir must talk to Mr Joe"...

Mr Joe is president of the company installing the machine

[robk]

Gcode, just forwarded the email to your other address. Please let me know when and/or if you have received it.

[MLS]

RobK,

 

That must be a machine or control specific thing because we use g02 and g03 with g43.4. No drill cycles as you stated earlier, but circle statements work fine.