Large Custom Form Helix/Thread On Lathe

[Mick]

I had someone ask me the other day, if Mastercam was capable of generating a threading toolpath on lathe, which would cut a large custom form thread using a turning tool like a neutral VBMT style insert. Imagine a large thread form where the tool makes individual passes following the form of the thread. The form is far too large to use a form tool.

My short answer, was no that it doesn't, but I'd be interested in feedback from anyone here on the board. He had been told that Edgecam and Surfcam could do it, though I'm not sure sure about that. This guy has Mastercam Lathe, and wants to use it to do this.

Has anyone here done something similar.

[JG]

Hi Mick,

I roughed a gear with a 64 deg ID helix (22 teeth) on a lathe using exactly the method you described. unfortunatly I did it by hand (kinda). I remember I used subs, one for the form of a single tooth that passed the start point of the contour for that pass, and i think i had one as a counter. I also used a vbmt style insert, although I had to tilt the tool into the helix for clearence. Due to the lead, I was only able to run about 50 rpm ~ 180 ipm, it was a lot of fun though.

 

now that I think about, I used MC for the 2d profile in the sub

 

Jg

[Philcott]

Mick,

 

Can you explain in a bit more detail what you want to do?

 

This is my guess.

 

Are you wanting to use a "V" insert which has a 35 deg included angle to cut a large thread? If so, I believe, you will end up having steps on the walls of the thread due to the angle on the insert being different from the thread angle. I take it you want to make rough cuts by stepping down in diameter as you alternate cutting on the front then the back edge of the thread. There is a feature in "thread cut parameters", "nc code format" called "alternating" this will cut on the front then back side of the thread groove but it relies on the inserts included angle to finish the walls.

I have not seen anywhere that allows you to cut a thread by walking down the cross sectional profile of the thread. Maybe someone else has.

 

Phil

[piergrid]

The thread profile has .6625 pitch and a .205 radius in the bottom and a .089 radius on top with 8 degree sides (16 included). Can this be profiled out with a form tool or a regular lathe tool ie. VBMT.

[Leandro]

Mick:

I already done something like this.

I set the start point of each thraedpass "manually" and my post generates just a "G33" pass, not a canned cycle.

For each pass I have a different operation.

A lot of work but works.

[rsbeadle]

I have done what you are talking about using a file from Mastercam, but I used the machine offsets to widen the thread to get what I wanted. I'm sure you could do it with multiple ops and get the same result. Make your thread program as you normally would in MC but split the middle of the desired thread width. Start and stop short by the amount of "movement" you need to get the desired width (I used a .236 grooving tool to cut a .750 wide spiral groove for coolant on a sleeve. Vary the offset plus and minus.257 in as big an increment as your machine can handle. Allow .257 at the beginning and the end). The trick is knowing your machine and making correct increments so that the profile of the groove/thread stays smooth. I also used a finish pass thread program and backed everything off and came in one cut at a time. My groove was .500/side deep and .750 wide in a thread form of 2.5inches per thread (.4 threads/inch). Hope this helps.

[gcode]

I've done this as well.

You program it like a multiple start thread.

 

You have to figure out the different Z values

to start the threading cycle.

 

For example

You are using a stub acme threading tool with a

.12 wide tip.

Do three threading cycles.

1 starting at Z.2

another at Z.15

and a third at Z .25

 

When its all over you'll have an Acme thread with a .220 wide root.

You can profile walls the same way, its just harder.

Draw a cross section of your thread and a cross section of your tool on the wall of the thread.

Then draw a 3d helix the diameter and pitch of the cut you want.

Draw it past the start of the part

Draw helixes for all the cuts you need and be sure to trim them all to the same plane.

 

The do a bunch of threading cycles with diameters

and Z starting point at the end of your helixes.

 

Its a good idea to prove your program out in aluminum. Mistakes can lead to some very heavy cuts. Its also easier to draw all this stuff

if you set you Z offset at the center of the tool

[Bruce Caulley]

Dejavu!!!!!!!!!

 

I did a tapered auger/ leadscrew years ago with a round turning insert. I did it in a different software, but I am sure that the method I used could be done in mastercam. It was sort of like a surface toolpath with threading cycles. 2134 of them

 

Actually reading Gcodes example I think it was pretty similar to what I did.

 

Bruce

[gcode]

quote:

---

I did it in a different software

---

If you had BobCad all you'd have to do is

"window it and cut it"

[jeff]

Mick,

Do youhave a fanuc comtrol?

And if so,does it allow for macros?

I have a macro that might help you out.

Let me know and I'll email it to ya.

[Mick]

Jeff,

 

Yes, its a Fanuc control on a DMG CT10 lathe. By all means, email it to me

 

Thankyou everyone for your responses. Everyone have assumed correctly. The way GCode described it, is the way I had considering doing it. The customer wants to use a VBMT insert to cut the shape. I'm visiting there tomorrow, so I will have a clearer idea. I'll take my camera, and take a photo of the job, and the lathe.

 

Thanks again for your prompt responses!

[Mick]

Jeff,

 

Yes, its a Fanuc control on a DMG CT10 lathe. By all means, email it to me

 

Thankyou everyone for your responses. Everyone have assumed correctly. The way GCode described it, is the way I had considering doing it. The customer wants to use a VBMT insert to cut the shape. I'm visiting there tomorrow, so I will have a clearer idea. I'll take my camera, and take a photo of the job, and the lathe.

 

Thanks again for your prompt responses!

[jeff]

Sent

[Bruce Caulley]

I have had a couple of requests fr a better description of how I did my augers.

 

 

Step1

NOTE: this was done on mill software not lathe.

 

Brown line is profile for 1 complete pitch.

Blue points are tip edge for a 6mm round insert for the “up” path.

Green points are for the down path.

 

Points are all the same distance apart in the X axis. (Z once coded for lathe)

 

 

 

 

 

Step 2

Up points have been transposed over to the X0.

Select these drill points from bottom to top and drill them.

Depending on how your settings or post is set up you will end up with something like :

G81 X Y blah blah blah….

G81 X Y blah blah blah….

G81 X Y blah blah blah….

G81 X Y blah blah blah….

G81 X Y blah blah blah….

 

It is then just a matter of doing a few copy and replaces to have a series of treading cycles that step up the profile. You then enter a U value in between each cycle equal to the amount that you have separated the points in the X axis above ( Z axis on lathe)

 

G76 blah blah blah

U0.2

G76 blah blah blah

U0.2

G76 blah blah blah

U0.2

G76 blah blah blah

 

The U may be positive or negative depending on the control. At the end of the up cycle repeat for the down side. At the end of the programme you must sum the U values and enter an amount to cancel this offset eg U-50.2 This is the end result.

 

 

I has been 5 years since I did these and I haven’t really used a lathe since, but hopefully I have put you on the right track.

 

Bruce

[Bruce Caulley]

Bugger. First couple of pictures don't show much. If any one wants them, email me.

 

Bruce

[Harryman]

Just a couple tools to throw into the toolbox here.

 

There is an editor called Textpad (not to be confused with Notepad) that has Block Edit mode, I'd call it collumnar edit. Textpad's ability to edit vertical collumns of text along with a spreadsheet's ability to produce collumns of G76s, Is, Js, Es, or whatever can be used to cobble together some interesting code.

 

Save spreadsheet as .prn (space delimited text file) it will open perfectly in an editor.