Is this possible?

> I'm having a problem getting this part made on our TL-1 for class. The part is a 5.500 long rod,with a .5625 radius on the end,followed by a 1.500 section that is .375 in diameter,the rest of the part is .500 dia. The radius on the end doesn't stop at 1/2 ball,it continues down to the .375 diameter,which is the problem. I have spent the biggest part of 4 days in class,and have yet to figure out how to make it cut a radius on the backside.

I was able to make a part that worked for him,by resetting the Z0 to where the nose radius stops,and plunging in to get the neck down to .375,but the backside of the nose has a chamfer that goes down to the .375 dia,instead of leaving a ball on the end of the part. Any ideas? Tommy D.

Of course it is possible. And really quite simple, once you see how. With cam, you can program the chain as a groove, and it will compensate the backside radius with whatever tool you choose. I believe you can also do this with the haas quickcode, but can't quite remember. Of course, you can always do the G-code by hand. Once you do the first side (face and full radius) with a od turning tool, and have 1.25 OD back to the 1.5" depth, load the groove tool and program a rough groove for your .375 diameter, rough the radius (you can do it with just straight cuts on X), then this simple contour:

G0 X1.2Z-.5 (RAPID CLOSE)
G1 X1.125 Z-.5625 (PLUS THE GROOVE TOOL WIDTH ON ALL -Z-'s)
G3 X.375 Z-1.0928 R.5625 (THEORETICAL SHARP INSERT CORNER)
G1 Z-1.5

Of course this is just a quickey - you should rough it out first, then this contour. And it has been a while since I've programmed a lathe, so verify on the graphics.

Basically it is the exact same as cutting the front radius, but you have to add the tool width since you will be using the backside of your tool. You can also use a left handed tool, and then it acts like your first tool, just the opposite. It would be harder though, since you need to rough out to the .375 diameter. Cam is nice because you can rough and finish to 1", then .75", and so on so your part stays much more stable. The 1.25 ball on the end of a 3/8 shaft will probably want to chatter a bunch.


Here is a haas pdf for the lathes. You should read through it before proceeding, as it will clarify what I scratched out here.

http://www.haascnc.com/training/LatheProgram_PDF/xlwb.pdf

> After reading your response,I realized I was unclear on a dimension. The ball on the end is .5625. The 1.500 section behind the ball isn't a diameter,but a length instead. The diameter of this section is .375,like an undercut. The remaining length of the part is .500 in diameter.

That shouldn't be that much different from what you describe,other than the finished dimensions being different. Thanks,Tommy D.

Your right, it isn't much different than what I described. I actually started out with .5625 as the diameter of the ball, then saw you had .5625 as a radius, so I changed it.

Try these (generic) numbers. Again - you need to add a negative _Z_ to all the actual Z's in this program to compensate for the fact that the back of the tool will be doing the cutting (cutter comp in Z, if you will)

G0 X.6 Z-.5 (RAPID CLOSE)
G1 X.5625 Z-.2812 (PLUS THE GROOVE TOOL WIDTH ON ALL -Z-'s)
G3 X.375 Z-4909 R.2812 (THEORETICAL SHARP INSERT CORNER)
G1 Z-1.9909 (THIS GETS YOU 1.5" FROM Z.4904 )


This should get you close - I can get you a actual program if you tell me what tool you are using. These are just like I said, pretty basic starting points.

Here would be a theoretical program with a .1" wide groove tool with sharp corners. Again, I am assuming you are roughing to .5625 diameter, and the front full radius is finished with your normal od turning tool.

G0 X.6 Z-.6
G1 X.5625 Z-.3812
G3 X.375 Z-4909 R.3812
G1 Z-2.0909

Notice the additional .1" only on the Z.

I assume this is basically the profile you are trying to achieve...

> Maybe I'll relate myself accurately for a change,LOL. You are right,the diameter of the ball is indeed .5625,making the radius .28125. The shank is 1.500 long x .375 dia. There is a .0625 long,45 degree chamfer at the back of the .375 diameter,the rest of the 5.500 overall length is .500 dia.

I have access to both MDJNR/L tool holders (DNMG insert),a 3/8 shank SDJCR with DCMT insert,2 different grade carbide insert threading tools,a square nose parting/grooving tool,and a .125 radius parting/grooving tool,both with carbide inserts. The SDJCR toolholder is mine,the rest of the stuff belongs to the school.

I also have various ground HSS tools,some of which would be eligible to be reground into a shape that works. I don't think insert tools with a 1/32 radius will work best here. The toolholder with the DCMT insert has a .0156 radius,and I have 2 inserts with .007.

I also have a set of 1/4 shank toolholders with a 60 degree triangle insert,all of these inserts have about .010 radius,and have several different insert alignments.

I've been envisioning getting this done with a 60 degree threading tool,but the instructor thinks the back edge of a DNMG insert will cause problems.

Since this part is not center-drilled in the ball,it will be done with about 2" sticking out of the chuck,so please no over-my-head depths of cut or insane feedrates.

If you have input on what tool I should be looking to use,feel free to help educate me. Hopefully,I have finally given you as clear a description as I can,which was entirely my fault. Thanks again in advance,Tommy D.

Tommy

Here is a code I've whipped up in a hurry.
You should be able to copy and paste it into the Haas, but remember one thing.
The code is written assuming an SL machine with turret behind the spindle. You may need to swap the X values if the TL requires negative direction.
Ditto for tool tip directions, so if a standard OD turning tool is Dir3, then all is well, but if the TL designates Dir2 for OD tools then you will need to swap the definition for tool3 to be:
Offset 03 = Dir2
Offset 13 = Dir1
That of course also mens that you need to exchange the comp directions as well.

This is a very good learning example from your teacher. Try to figure out what my code does and make sense of it. Try to figure out some of the minor details and why they are where and how they are.
Of course, feel free to ask any questions.

Oh, I took liberty and gave you a VNMG tool for roughing the back. The DNMG just don't have enough back angle to do too much good, and would leave quite a bit of material for your TL to take out on the finish pass.
Naturally, if you have a groove-turn tool, you can use that, but I'll leave it for you to figure out what edge to pick up in the offsets.



%
O00100
(TOMMY-D - BALLEND)
(DATE - TODAY)
(OPERATION - ROUGH AND FINISH BALL END)
(ASSUMING 1 3/8 STOCK DIA)
(CYCLE TIME: )
(ROUGH FRONT - DNMG)
G54
G28
G50 S1000
G00 G97 T101 S600 M03
G00 X1.4 Z0
G96 S300 M08
G01 X-.04 F.006
G00 X1.375 Z0.05
G71 D.05 P100 Q150 U.008 W.003 F.006
N100 G00 X0.
G01 X0. Z0.
G03 X1.125 Z-0.5625 R0.5625
G01 X1.125 Z-0.6625
N150 G01 X1.375 Z-0.6625
M09
G28
(ROUGH BEHIND BALL - VNMG)
G00 G97 T202 S600 M03
G00 G42 X1.375 Z-0.4625
G96 S300 M08
G71 D.03 P200 Q250 U.008 W0 F.004
N200 G01 X1.125 Z-0.4625
G01 X1.125 Z-0.5625
G03 X0.7955 Z-0.9602 R0.5625
G01 X0.375 Z-1.1705
G01 X0.375 Z-2.625
N250 G01 X1.375 Z-2.625
G00 G40 X1.5 Z.1
M09
G28
(FINISH FRONT AND BACK, .125 GROOVING TOOL)
(OFFSET 03=DIR3, 13=DIR4)
G00 G97 T303 S600 M03
(START WITH SHOULDER, THEN FRONT OF BALL)
G00 G41 X1.525 Z-2.625
G96 S300 M08
G01 X0.375 Z-2.625 F.002
G01 X0.375 Z-1.625
G01 G40 X1.525 Z-1.625 F.05
G01 G41 X1.525 Z-0.7625
G01 X1.125 Z-0.7625 F.002
G01 X1.125 Z-0.5625
G02 X0. Z0. R0.5625
G01 X-0.4 Z0.
G01 G40 X-0.4 Z0.2 F.05
G01 X1.525 F.2
T313 (CHANGE TOOL TIP DIR)
(TO FINISH BACK OF BALL)
G01 G42 X1.525 Z-0.3625
G01 X1.125 Z-0.3625 F.002
G01 X1.125 Z-0.5625
G03 X0.375 Z-1.0928 R0.5625
G01 X0.375 Z-1.825
G01 G40 X1.525 Z-1.825 F.05
M09
M05
G28
T101
M30
%