help with turning tool offset

[Shizzlemah]

Guys, I know this may be a simple question but I am having a real bugger of a time setting tool diameter comp properly.

In the past, I have never been able to get the control to properly deal with tool tip radius. No problem if it is a dead sharp tool w/o comp, but the radius never seems to be compensated correctly.

Doing spherical parts, they always come out egg shaped with a nub on the front. I recall it not dealing well with coming in at a negative X to start facing. I am pretty sure that I am doing something wrong, so I post here in hopes that someone can point me to the procedure for setting up & using comp.

In the past, I have used centerline programming w/o comp and that has allowed me to cheat.

However, I now need to run a part that will be rouged with a .032" rad tool and finished with a .016" rad tool. I'd love to use the G71/2 roughing with the .032"R and just chase it with G70 finishing & .016"R.

The specific part/feature is simple enough to think of as a spherical end on a piece of barstock. Lots of roughing.

Any pointers?

When setting tool offsets, I touch X to 1" diam stock (example) and set the X offset to 1.00 and 'measure'. Then touch the end of the stock, Z offset to 0.00 and 'measure'. Then I key in the radius offset as what ever it is. And always set the wear offsets to zero and check that the tool nose vector is correct. Set all the tools to the same Z0, then later set the part Z0 referencing a tool.

Any help greatly appreciated ! ! ! Surely someone has run radius comp sucessfully on a lathe!

[Geof]

I am not sure I can help but one thing I did discover when trying to use tool comp and G71 on a Haas is that the canned cycle ignores the tool comp command if it is in the P-Q blocks. I faked it by making the U value larger than the tool nose radius so the roughing cycle left enough material for a finishing cut. I will have to check the program but I think I had to repeat the coordinates and do the finish cut outside of any canned cycle. I can post the program if you like.

I am currently working on setting up programs for making 2" to 3.4" spheres by machining everything except a 1" diameter neck then fixturing them in a sort of shopmade spherical collet to remove the neck and finish the sphere. My goal is to have the final sphere including the blend round to within less than 0.0005" and then I will finish the final bit by polishing on a ball generating machine (I hope).

If all goes well the next thing is hollow spheres with a wall thickness of around 0.15".

[camtd]

Hi

I was wondering how tech support is for this control? In a job shop atmosphere I need to get information the same day. Does this happen with this company?

Thank You

[HuFlungDung]

Shizzlemah,

If you are actually machining more than a hemispherical ball end, then you will actually have to shift comp modes at the max X of the ball from right to left. I do not have any experience with using comp in lathe cycles, but there has to be that much restriction in the use of it, ie., X must continuously increase or decrease along one path, same for Z.

[Shizzlemah]

Hu-
Good point.

From the centroid manual : "G42 offsets the tool ... the amount of its nose radius to the right of the workpiece relative to the direction of travel."

The crummy sketches show G41/Left comp for turning OD away from the chuck, and G42/Right for OD turning toward the chuck.

Is that restriction also in Z ? When trying a hemispherical end, the closest I could get to round would leave a flat spot on the end of the stock. The diam of the flat was equal to 2x the nose radius. Meaning it came in comped to X0... Where it should have comp'd to X=-radius.

[CNCRim]

Best way to program is with no radius on the tool, just program exactly what you see on the print and use G41 or G42 depend on the relation to the vector.

Shizzlmah, can you post your program on here we can take a look at this, that way we have a better idea what you want. There are 3 way to program and setup, the program and the tool offset must be match, otherwise the sphere won't come out right. I can post a program if you like.

[HuFlungDung]

Shiz,
I'm all wet. I did a sample toolpath in OneCNC and it does not switch comp modes halfway around the circle.

I was reading my Mits manual and it talks about setting the vector for the tool. Now this vector setting is new to me, so I'm interested in hearing how this is supposed to work. It all seems a bit ambiguous at this point.

BTW, are you using a ball type toolnose, or a bullnose type where the cutting switches sides on the insert?

[Shizzlemah]

Newtexas-
Do you mean program the shape of the print, then use the tool offsets to set diam offset, then apply G41/2 to suit ? That is exactly what I am trying to do. Using the centroid conversational, and it's giving me footballs with a little nub on the end (nub diam = 2 times tool nose rad!)
I can tweak the G3 Z & R values to try and make it look more round, but that isn't going to cut it on this job.

I would love to see some sample code to get me moving in the right direction.

Ok more details. I want to use the G71(rough profile) and G70(finish profile) to put a hemisphere on the end of a piece of stock.

The stock in this case is hard 17-4, about 36Rc. I want to rough the profile with a cheap trigon carbide insert, then a finish pass with a pricey, delicate 35deg diamond shaped ceramic insert. The trigon is .032" radius, diamond is .016" radius.

In the past, I have got around this by just centerline programming the profile, using G40 (no comp) and could then run it with a G71 rough/ G70 finish.
But since the rough & finish tools here have different radii, that approach will not work.

I have 38 different parts to program - all very similar in style with different dims on the ball end. I don't want to be at the console punching, tweaking, and scrapping parts!

I think I am gonna try :

T0101 (rough trigon)
G71 P10 Q20 (rough profile cycle)
N10 G41
N11 (profile here)
N20 G40
G28
T0202 (finish diamond)
G70 P10 Q20 (finish profile)

I think this way, calling the G41 right in the cycle, I may have a better chance. Of course the profile will now need to contain entry/exit moves, but this seems like the best hiar-brained idea yet.

Any sample code is greatly appreciated.

[CNCRim]

A sample of 1" sphere rad.

Program with 0Rad is so much easier to calculate.........
Program with G41/G42 and 0Rad:
G20
(TOOL - 1 OFFSET - 1)
(80 DEG. INSERT - CNMG-432)
(ROUGH)
G0T0101
G18
G97S382M3
G0G54X2.Z0.1
G50S2000
G96S200
G71U.1R0.
G71P1Q3U.02W.01F.006(Note: some control has difference format G71P1Q3U.02W.01D.1F.006)
N1G0X-.06(**Start**)
G1Z0F.005
X0
G3X2.Z-1.R1.F.01
N3G1Z-1.03(**end**)
G0Z0.1
G28U0.V0.W0.M05
M01
(TOOL - 2 OFFSET - 2)
(35 DEG. INSERT - VNMG-431)
(FINISH)
G0T0202
G18
G97S3600M3
G0G54X2.Z0.1
G50S2000
G96S200
G41
G70P1Q3
G40
G0Z0.1
G28U0.V0.W0.M05
M30



Program without comp and .0312Rad: (Can't not use G41/G42 or else)
(TOOL - 1 OFFSET - 1)
(35 DEG. INSERT - VNMG-432)
(.0313RAD)
G0T0101
G18
G97S3600M13
G0G54X-.0625Z.1
G50S3600
G96S200
G99G1Z0.F.01
G3X2.Z-1.0313R1.0313
G0X2.1414Z-.9605
G28U0.V0.W0.M05
M01

Program without comp and .0156Rad: (Can't not use G41/G42 or else)
(TOOL - 2 OFFSET - 2)
(35 DEG. INSERT - VNMG-431)
(.0156RAD)
G0T0202
G18
G97S3600M13
G0G54X-.0313Z.1
G50S3600
G96S200
G1Z0.F.01
G3X2.Z-1.0156R1.0156
G0X2.1414Z-.9449
G28U0.V0.W0.M05
M1


Cheers,
Hope it will help!

[Shizzlemah]

Newtexas,
Your first sample is right along what I want to do. G71 rough, G70 finish. All dimensions in the program are taken right off the print.
But where do you call the G41/42 comp ?

Would it go right after N1, or right after the T tool change ?

Thank you!

[CNCRim]

G41/G42 get call on the finish tool. The control will inogre cutter comp under G71 and G72.