Quick question on 4th Axis G-Code

[CJH]

I have a quick question that I'm hoping to get answered. Our CAM software vendor is working on tweeking a Haas post for us and sent me a question about how the code should read.

This was his question........Does the machine need to have an <axis>0 on every move line or is it a modal command so it only needs to come out once?


If anyone knows the answer to this it would be helpful. We have a techgnician coming shortly to set up our 4th axis unit, but still don't have a working post for it.

CJH

[tstom]

Not sure why a Haas would be different but the machines we have the post only outputs an A axis value when it needs the rotary to move

I'm not a Haas expert though...have him set it up and do an "air cut" well above everything to see what happens

[CJH]

Thanks...

I'm hoping the tech brings a few sample programs to use to train us with. The reason i'm asking the question is that we are having 2 posts set up. One will do index moves like cutting at A0 the turn to say 90, 180, 270. The other will do wrap moves to cut in full rotation simultaneously. We are using a couple of different CAM programs and none have the licenses as of yet to do full 4th axis work. this is basically to just get us started so we can use the unit.

[Geof]

If you mean you want the rotary axis to go to A0. and stay there you just do not program any A commands until you want it to move to a different position then you give it A90. and it moves to 90. and stays there until you give a different position. It is like any axis, it stays at the last commanded position.

You should also read your manual on "Quick Rotary G28" so you can figure out how to save time returning the A axis to zero without having to unwind all your previous moves when you go past A360.

[CJH]

Geof,

Yeah that's pretty much much what I think I meant. We would start out at cutting in one "A" angle Then we would want to index to the next like say A90. So I would think the rotary would only need to have the next angle to turn to showing up once, if it is merely doing index turns to machine at the next location. Is this correct? So I guess that what your telling me is that the moves are modal. Am I right? I don't want to sound stupid, but machining with an automated rotary is completely new to me. I've done stuff on a manual index head on our mill.

So here is the next question. If we want to machine a cylinder or similar continuously, does the code to need to have the A position on the end of each line?

Again not wanting to ask stupid questions. I know I need to dig into the manual a bit, and also pay close attention when the tech is in. I'm just trying to learn a little so that I ask the right questions. Afterall that's why I read this forum since all of the guys on here seem to have some really good expirience and don't mind sharing knowledge.

[Geof]

You have it correct. To machine the A0. face of something you need the command G00 A0. and follow this with all your program, then A90. followed by the program for the A90. face etc.

The easy way is to make the program a subroutine so you do G00 A0. M97 P(line number), and start your entire program at that line number. Like this:

G00 A0.
M97 P1000
G00 A90.
M07 P1000
G00 A180.
M97 P1000
;
;
;
M30
N1000
Your program
M99

Of course I have left a lot out.

Calling it modal is not quite correct because modal applies to the G command such as G00, G01 etc but what you are doing is positioning an axis which will stay at that position until you tell it to move further on in the program.

For moving the A axis at the same time as a linear axis you just include it in the command.

G01 A720. X-10. F(something)

Will rotate the A axis through two revolutions while moving X -10." so you could cut a helix.

[tstom]

[QUOTE


So here is the next question. If we want to machine a cylinder or similar continuously, does the code to need to have the A position on the end of each line?

QUOTE]


Yes ,that is correct how ever in Mastercam at least you do not need two different posts the correct post will do indexing and continous 4 axis milling

[CJH]

Geof,

This is helpful. Our technician actually showed up today, since he lives in the area to do the install for us. fortunately our software vendor was able to send down some sample code. It didn't look anything like what you jotted down for me. Of course I hadn't seen your reply till after the tech had left.
When he was in the shop, he looked at the sample code from our vendor and couldn't make sense of it, and didn't have any suggestions other than to call Haas and have them look at it. He said he was not a programmer and only knew the basics. So I sent the sample gode to our machine dealer to get help and the tech/programmer there was able to get to the root of what I was trying to describe in probably a backwards manner over the phone. I'm going to test it on Monday. But what he sent back to me as modified code, was more in line with the sample that you posted in your reply.

There is one thing that I was curious about and forgot ask the service installer. I had made a forum post a while back similar to this to ask about the same stuff. I had read i think in one of the replies, or in another forum thread altogether that the Haas control will only accept 1 dia. for the stock, so it should be the max dia. What I forgot to ask was where do we enter that in the control. Can you point to an answer. I am going to assume here and correct me if I am wrong.....The zeros for the axes will be X0 at our descretion on either end of the stock depending on how we have it set up in our cam program, the Y0 will be dead center of the rotary axis, and the Z0 will also be dead center on the rotary. So the question is where would we would enter in the dia. of the part stock? I looked for something in the rotary manual and didn't seem to see anything.

Tstom,

Yeah I now Mastercam will do both with only one post. We just bought that with our new router from Onsrud. I haven't used it yet. But since Artcam is only a 3 axis software we need the post to fake the rotary moves to get what we want. Were porbably going to get the 4th axis license for MC soon, it's just a matter of funds and justification to managmment.

I'll keep ya posted on our progress, thanks for the help.

CJH

[RMACSHOP]

The Haas also has a code for Cylindrical mapping were you can change one of your axis to trade moves with the x or y axis.(I dont remember the code off the top of my head but it is a G code G107 I think) You also put your dia. of the part you are machining in the form of a R(radius of your part).You can also leave The R out and set the dia. in the settings. So you can program the part as if it was a square part and the machine will automaticly map the part with the dia.

So at the beginning of your tool it would read
G107 A0 Y0(using the A and Y axis) R(radius of workpiece)
A0 X0(if you want to use A and X axis)
At the end of your tool use the G107 to turn off Cylindrical mapping

This will only work with a haas interface on your fourth

I dont know if this helps but I have quite a few Haas machines and we do not use any software to program anything unles it is a 3D part. we believe it is just faster. We can answer just about any question you have about the Haas programming codes. I hope this helps some.

RMACSHOP

[Geof]

Originally Posted by CJH .... the Haas control will only accept 1 dia. for the stock, so it should be the max dia.... So the question is where would we would enter in the dia. of the part stock? I looked for something in the rotary manual and didn't seem to see anything...CJH

Read all about G107 in your mill manual; this may help...but it may not because it is written in such a convoluted manner.

[CJH]

Thanks Geof, I found what I was looking for.

CJH