Lathe live tooling issues

[ty]

Hi All,

I've been a lurker here for quite some time and have learned a lot, and been in awe of the knowledge seen on this board. Thank you for all I have learned so far.

We (ICE Prototyping) are a small rapid prototyping company in San Antonio, TX. We have a Haas SL 20 lathe and a VF2 mill. I am the machinist due to the needs of the company, NOT by trade! I am learning as I go, and the help of this board and a friendly machinist in Victoria has made most of my ventures a (slow) success.

I am doing a simple live tooling operation to put two flats on a .328 round part. The flats are for a 1/4" wrench. The part comes out with a "hump" in the middle of what is supposed to be flat. It seems to me that I may have a resolution issue, but I know VERY little about these things. Below you will find the guts of the code. I find it interesting that only four X moves are required to interpolate the flat as the part rotates, but I'm just a recovering idiot in the world of CNC.

Thank you in advance for any help that I may gain here.

ps, Mastercam rocks!

ty

N110 G0 T0303 ( 1/4 FLAT ENDMILL )

N112 M154

N114 M133 P777

N116 M8

N118 G0 X.6238 Z.1 C126.723

N120 G1 Z-.35 F22.

N122 X.598 C123.265 F.1

N124 X.5953 C57.138

N126 X.6208 C53.647

N128 G0 Z-.25

N130 Z.1

N132 C-53.647

N134 G1 Z-.35 F22.

N136 X.5953 C-57.138 F.1

N138 X.598 C-123.265

N140 X.6238 C-126.723

N142 G0 Z-.25

N144 M135

N146 M155

N148 M9

[Philcott]

Ty,

 

When I am cutting wrench flats on the outside of a turned part, I almost always use a woodruff cutter and interpolate around the part in polar notching mode (G112) on our Mori. This will give you good flats. The only drawback is you need to have enough clearance height between the cutter diameter and the shank and the od of the part.

 

I am leaving in 20 minutes for a week off but I am sure some of the other boys will chime in and give you a hand.

 

Good luck,

 

Phil

 

PS. The "C" moves are your chuck rotation, I believe it's the "X" moves that are giving you your bump on the flats.

[crazy^millman]

If you want to only put 2 flat then that is a ton of code I would think you would have one line for the 1st side and cleracne move then an index move of the spindle then one more move and then another cleracne move and home and done. How about outting pu the file of the FTP and let some of the Lathe guys take a look I personally think you got soemthing going on that might be givingyou this probelm and without seeing the files a really big guess at this point.

 

This is just my opinion and use it at your own caution. Have a nice day.

[ty]

Thanks Phil. Enjoy the time off.

 

Stupid question (see first post refering to me as an idiot), but does Mastercam handle that for you or is this a manual thing?

I am under the impression that our post should bust out everthing needed for this operation.

ty

[crazy^millman]

Well I think it would depend on the operation you are using and how you are using it. I dont know how the machine is set-up so I can only guess.

[ty]

Millman crazy,

I think MORE code is required because the movement has to be interpolated as the tool is on the centerline axis of the part.....

[Philcott]

Mastercam will do it for you. Go to toolpaths, next menu, c-axis, face contour. (you will have had to draw the contour first using the side view) Select chain, and go from there. Be aware you will probably need to turn on Mi2 or Mi4 to activate the polar notching in your post. Open the post file (in cimco edit) and read the instructions at the top of the file regarding polar notching.

 

Chris, mill/turn, and others should be here soon.

 

Phil

[crazy^millman]

Yeah if the tool does not travel and it stationary then yes you would need that I am thinking you would go at it with the Z travel verse trying to travel the y axis if on a lathe. If needing to do it the X axis then you would need exactly what you are thinking and I thin kthe woodruff cutter might give you better clearence if you could fit it in there.

[ty]

Phil,

I had you up to "be aware". I haven't ever turned on the Mi2, mostly because I never heard of it.

 

 

ignorant, but very willing to learn.

[Don S at Barefoot CNC South]

Hi all,

TY this what I got when I posted it face contour

1/4 flat on .328 dia. 1/2 deep.

 

code

(TOOL - 1 OFFSET - 1)

(FACE CONTOUR 3/8 FLAT ENDMILL)

G0T0101

M18

G0G54X.9943Z.1

C14.563

M8

G97S1426M04

G98G1Z-.5F6.33

G98G1G12.1

G42X.2123C.125

X-.2123

G40X-.9623

Z-.4F500.

Z.1

C-.125

Z-.5F6.33

G42X-.2123

X.2123

G13.1

G40X.9943C345.437F570.03

G0Z-.4

M9

G00X8.Z8.H0.M05

T0100

M30

 

HTH

Don S

[CNCGUY]

quote:

---

I had you up to "be aware". I haven't ever turned on the Mi2, mostly because I never heard of it.

---

Mi = Misc Integers

 

In the op that you have cutting the wrench flats, click on Tool parameters then Misc values.

 

In there you should find

code:

---

 Mill Cycle G107/G112 [0=OFF,1/-1=ON] 

---

turn this on to get the G112 code you need.

 

HTH

[chris m]

Not all live-tool lathes are shipped with co-ordinate system conversion [my Okuma LT doesn't have it 'cause they didn't want to pay for it; BIG MISTAKE, BTW] but if your Haas has it [look in the book to see if it has the same configuration as a Fanuc, it probably does] and you're using MPLFAN as a your post you'll need mi4, I believe:

 

#mi4 = Canned conversion cycle type selection:

# Mill-

# Activates milling axis conversation canned cycles (G107 or G112).

# 1 or -1 activates the cycle, the path continues until next entry is

# zero, sign switches (1 to -1) forces g113 at null toolchnge, the

# cycle changes or the tool changes.

 

Which should give you very concise code to generate what you want.

 

Not at all trying to be a wiseass; did you call Applications at your HFO? They should be able to help you out in no time; at least to manually program the part to get it going.

 

C

[ty]

Thanks all. I will look into all of this and post the results. I really appreciate the time you have spent so far helping me out.

I've sent emails to the distributer that wrote our posts, just waiting for a reply...

ty

[ty]

Well, the pressure switch went south so i guess I'll resume my efforts Monday...

[LNDCAD]

I have done the same thing on HAAS SL turning centers and the solution that I found is to use a woodruff cutter, or if you need more clearance to the cutter shank, or a longer reach (flats closer to the chuck than the face) you can use a slitting saw blade on a live tool arbor and a face contour command. If you use a flat endmill with a cross contour, you will get a hump in the middle of the flat, since the machine control is trying to drive a flat face cutter around a profile using X and C moves. Even if you break the cut into many X and C moves, the edges of the cutter will undercut as you move away from the center of the flat. I uploaded a file SAW FLATS TEST.MC9 to the Unspecified Uploads Directory on cadcam's FTP site. It shows an example of both a face and cross contour on a lathe. HTH.

[Tim Johnson]

I don't know much about HASS but if you are driving your toolpath on flat geometry it should come out flat. Another idea is your cutter in not at the vurtual "Y" center because of the tool holder or maybe a crash moved the turret or spindle. We've had both problems on our 3 axis lathes. Indicate the holder to the center of the spindle to make sure your holder is concentric to the spindle. If it's off perpendicular to the x axis, indicate the turret along the x axis to make sure it hasn't moved. If the turret is fine but you have to shim your lathe holders to make a facing tool cut to the center cleanly, it could be the spindle has been moved.

 

Hopefully it is the toolpath