Newbie Haas OL-1 User (CNC Lathe)

[Jorge-D-Fuentes]

This computer was not supplied with anything but the most basic of programs, and uses that panel keyboard, and it's kinda setting my boss on fire.

I'm wondering if there's a better way to do the profiling for the CNC, one that doesn't make us pull our hair out.

I'm used to working with Rhino3D, but none of the software plugins/packages I've researched seem to be Lathe-oriented (RhinoCAM looks like it's for Milling, and so do other programs like MetaCut Utilities and Teksoft).

It's just a Lathe... I should be able to take a cross-section of what I'm doing and turn it into the five or so lines, and feed it to the machine without hassle...

I'm absolutely new with G-Code, and it's painful to have to go to the machine's built-in DOS-looking editor and type G54 X-- Z--, etc. etc.

I just wanna design Rings (we designs Rings here, but they're plain bands, not intricate jewelry like what you would need something like MATRIX for or anything).

So... yeah... is there a better way? Preferrably one that involves Rhino?

Thanks.

Sincerely,
Jorge

[Bluesman]

Originally Posted by Jorge-D-Fuentes This computer was not supplied with anything but the most basic of programs, and uses that panel keyboard, and it's kinda setting my boss on fire. I'm wondering if there's a better way to do the profiling for the CNC, one that doesn't make us pull our hair out. I'm used to working with Rhino3D, but none of the software plugins/packages I've researched seem to be Lathe-oriented (RhinoCAM looks like it's for Milling, and so do other programs like MetaCut Utilities and Teksoft). It's just a Lathe... I should be able to take a cross-section of what I'm doing and turn it into the five or so lines, and feed it to the machine without hassle... I'm absolutely new with G-Code, and it's painful to have to go to the machine's built-in DOS-looking editor and type G54 X-- Z--, etc. etc. I just wanna design Rings (we designs Rings here, but they're plain bands, not intricate jewelry like what you would need something like MATRIX for or anything). So... yeah... is there a better way? Preferrably one that involves Rhino? Thanks. Sincerely, Jorge

HAAS is pretty easy to program, I am not sure how old your control is but her is a link to a woorkbook in PFD format, I would e-mail you my copy but it is to big a file to send. So this may help you get started

http://www.haascnc.com/training/Lath...m_PDF/xlwb.pdf


Bluesman

[Geof]

Jorge;

Do you have any pictures, cross sections with dimensions, of the type of thing you want to turn. It is difficult to understand what is so painful about typing a few lines without seeing what the few lines are supposed to do.

[Jorge-D-Fuentes]

I guess I just felt there was a nice program out there that could take a drawing and turn it into code so that I wouldn't have to learn it.

I guess there isn't.

I figured out the basic template of what to do, but I gotta learn all the G-codes and how they work.

The machine broke on Friday, so I've a few days to figure it out. (the rod that holds the chuck 'fell out' somehow... I guess when Haas came here and built the machine, they had that either loose or a bit too far out).

[gilchapa]

When we bought our first NC machine we used BOBCAD. Its the best for newbies.

www.bobcad.com

Its very cheap too, but that doesnt make it any less good.

[Jorge-D-Fuentes]

We just had a bad experience with the Bobcad people. Apparently, Bobcad doesn't have a visual representation of the Turning functions, which turned off my Boss, but the worst part was that after the online/phone presentation, the bobcad guy immediately put us on the phone with a Salesman, who started to pitch the thing down our throat.

If it can't simulate turning and provide an Accurate G-Code, it's no good to us, pretty much.

Bobcad looks good for simulating Milling, and only milling of a straight piece. We work with Rings, so we use milling machines that have servo motors or hi-velocity spindles, so if it can't simulate at least the cutting of the stock in Lathe Mode, then it's not worth Buying.

Now VisualTurn has a little more potential in that it shows you (after the painful "Tool Definition" stuff) the stock and the cutting. The problem with that program is that it's crippled, and we don't want to buy a $1000 if the G-Code it generates is incorrect or inaccurate.

Going back to the machine itself, I've been successful in generating "Part Surface" G-Code (that is, G-code that represents the part contour, without tool compensation), and I told these people (my superiors) that the part won't be accurate until Tool Nose Compensation is used (we're working with very small pieces here, inch in diameter, .165" in width), but they told me to do it without it.

Now I did it without it, and they tell me to learn how to use it. Mlargh (I'm just venting now).

On top of that, we still seem to be having issues setting up the Tools. When the guy who set the machine up showed up, it took him maybe 1/2hr to set up all three tools (facing/toptrim tool, InsideRounding tool, PartingOff tool), and the guy who's here setting them up now (we had to reset the Zero point for a standard for all G-Code programming people) doesn't seem to know what he's doing. Not that I know all that much either, but he's kinda doing the whole "Don't get in my way" thing.

He's been going at it since Friday afternoon.

Sorry... venting again...

Well, basically I just gotta implement the G40,41, and 42 codes intelligently in my programs so that the rings' top trimming is even-looking and it parts the ring in the same place. Although for this, I gotta wait until this guy sets the tools up... mlargh...

[gripper]

Hi
If you post a drawing of what you want to make, I'll write you a program that you can use as a template if it's just rings. The program will contain this, bar stop, rough turn, spot face, drill, bore, finish turn and part off, or what ever it takes to make your bit. it will be writen in fanuc G-code if thats any use and contain the offset commands. I do this most days, I program by hand at the machine. If theres any thing else just ask and we'll try to help.

[gilchapa]

MasterCAM has a very good simulation tool for lathe, and with the correct post processors it will give you the code you want every time.

If you are writing programs for making simple parts (like rings), that come from a standard source (like a bar) I wouldnt bother buying a CAM package and do all the programming by hand in the machine. It will take you some time to figure out to know how to do what you want, but with some practice it will be very easy.

On a more personal note, tell your boss to relax, he'll get a heart attack (or is it a she?) Learning always takes some time, and a new machine, always has some learning involved.

[Jorge-D-Fuentes]

Truthfully, I'm the one that's stressed out, as I wanna get this stuff going right away.

Okay, I'm gonna upload a G-Code example I did on my own, and I'll also upload a Rhino representation. Hopefully the sample is understandable:



////////////////////////////////////////////////////
%
O00600 (LD040-0600)
G18 G20 G40 G64 G80 G97 G99

(WARNING- SET MACHINE 654 FIRST)

G53 G00 Z-2.000 T0 (MACHINE MOVEMENT)
T101 (SWITCHING TO TTR/FACE Tool)
G97 S3500 M03

G54 G00 X1.100 M08 (RAPID TO 1.1DIA)
Z0.400 (RAPID LEFT TO 0.5)
G01 Z0.165 F0.006 (RAPID LEFT AGAIN TO FACING POINT)
G01 X0.500 (FACING)
G00 X1.100 Z0.165 (RAPID RETURN)

X0.761 Z0.250 (RIGHT OF START OF T-ARC1)
G01 Z0.165 F0.002 (T-ARC1 START POINT)
G03 Z0.000 R0.138 (CCW T-ARC1)
G01 Z-0.037 (LEFT FOR PARTING HELP)
G00 X1.100 (RAPID OUTWARDS TO SAFEZONE)
Z0.400 (RAPID RIGHT)

X0.721 Z0.250 (RIGHT OF START OF T-ARC2)
G01 Z0.165 F0.002 (T-ARC2 START POINT)
G03 Z0.000 R0.138 (CCW T-ARC2)
G01 Z-0.037 (LEFT FOR PARTING HELP)
G00 X1.100 (RAPID OUTWARDS TO SAFEZONE)
Z0.400 (RAPID RIGHT)

X0.681 Z0.250 (RIGHT OF START OF T-ARC3)
G01 Z0.165 F0.002 (T-ARC3 START POINT)
G03 Z0.000 R0.138 (CCW T-ARC3)
G01 Z-0.037 (LEFT FOR PARTING HELP)
G00 X1.100 (RAPID OUTWARDS TO SAFEZONE)
Z0.400 (RAPID RIGHT)

G53 G00 Z-2.000 T0 (MACHINE MOVEMENT)

T202 (SWITCH TO IR TOOL)
G00 G54 X1.100 (RAPID TO 1.1DIA)
Z0.400 (RAPID LEFT TO 0.5)
G00 Z0.250 (RAPID LEFT AGAIN TO 0.250)

X0.607 (DOWN TO RIGHT OF START OR I-CUT1)
G01 Z0.165 F0.006 (I-CUT1 START POINT)
G01 Z0.000 (INSIDE CUT1)
G00 X0.500 (RAPID INWARDS TO SAFEZONE)
Z0.250 (RAPID RIGHT)

X0.647 (RIGHT OF START OF I-CUT2)
G01 Z0.165 (I-CUT2 START POING)
G01 Z0.000 (INSIDE CUT2)
G00 X0.500 (RAPID INWARDS TO SAFEZONE)
Z0.250 (RAPID RIGHT)

G53 G00 Z-2.000 T0 (MACHINE MOVEMENT)

T303 (SWITCH TO PART-OFF TOOL)
G00 G54 X1.100 M08 (RAPID TO 1.1DIA)
M03 G97 S3500 (SPINDLE STUFF)
G00 Z-0.037 (SLOW LEFT TO PART-OFF [P-CATCHER!])
G01 X0.500 F0.015 (PARTING- [P-CATCHER!])
G00 X1.1 (RAPID RETURN TO SAFEZONE)
(HOPEFULLY PARTS-CATCHER CATCHES RING ON RAPID)
Z0.400 (RAPID RIGHT TO SAFEZONE)
M09 (TURN COOLANT OFF)
G53 G00 Z-2.000 T0 (MACHINE MOVEMENT)

M30 (PROGRAM END + REWIND)
%
//////////////////////////////////////////////

Okay, explanation:
We have three tools, a facing/top-trim tool (Diamond-shaped), an Inside-Round (I guess kinda like a threading) tool, and a thin Parting-Off Tool.

Now, the G-Code described above I did by learning from the HAAS examples, and by studying the first code, given by the programmer who set the machine.

Also, you'll notice it does NOT use Tool compensation (G41,42... and I think this might come back and hurt us later).

The parting off tool is 0.037", which is why there's a left movement after the arcs, to give that last tool a 'place' to cut, so that there's very little material left.

As for the Stock (which is not shown here), it's generally 0.010-0.015" larger than the top trim and smaller than the inside round.

The rings are not coming out correct, and I fear that it's because of the lack of Tool Compensation.

[Geof]

I just ran your program in graphics on a Haas lathe and there are no problems with it as far as I can tell. With the correct tools you should get the rings off correctly.

I do notice in your post this: "We have three tools, a facing/top-trim tool (Diamond-shaped), .......".

The tool you use for facing is not suitable for turning the OD profile. A facing tool has to be positioned in a 'handed' manner for front or back facing but your profile tool needs to be positioned symmetrically. I have uploaded a sketch showing this. I think all you need to do is put in a tool for the OD profile that is positioned as shown and you will get symmetric rings.

It is not necessary to use tool compensation but you will have to take into account the tool nose radius in your coordinates.

[Jorge-D-Fuentes]

Image here:
(Pretend the Ring is under this image to get a sense of where it's gonna cut and how)


As you can see (oh, the image is in Mils [Thousands of an Inch]), we've got thoat 0.008" that we've not been compensating.

On top of that, the tool orientation is a bit off.

Lastly, we're not working with a bar cylinder, but rather with small blanks, about 0.4" in width and 1" in outer Diameter (0.6" inner diameter). I'm concerned that if they get a tool that is symmetrically oriented, there may be some problems working with such thin pieces.

But yeah, I figured there was a solution that could be done, and compensating in the program for the cutter Radius would definitely help. I don't like that the tool (101) is oriented how it is, but I don't know if my boss is planning on getting a fourth tool any time soon.

[PBMW]

I don't mean this in an unkind way...But after the investment of 40 grand or so...your boss may want to think about hireing a machinist...