[fordav11]

Looking to buy MC X current version. Just wondering if Mastercam can generate special threads using a single point tool? For example a thread with 20 degrees front angle and 45 degrees back angle with a 0.1" rad at the bottom by 0.25" deep using a common PDPNN tool with DNMG insert and multiple G92 lines? I remember inquiring directly to Mastercam a few years back (around when MC X was released) and they said it was planned but not a priority. I don't need anything else from any CAM software except this. The rest I can do on the machine
We do it now using Autocad and manually work out the cuts but it's a PITA
Is there any better solution (or any solution?) for auto-generating special threads?

[Mike Mattera]

Mastercam will do helical motion to create a thread. The shape is determined by the insert. I dont see any reason Mastercam wouldn't do what you want.

Mike

[WallyL7]

I believe he is referring to lathe threads.

If it is a canned G71 type code that your machine reads a bunch of different variables, then I think you should be able to do it. You do need to have the correct post to control what goes where though.

It may depend more on the machine's thread cycle. What machine is it? And again, are you already doing all this with one canned cycle?

[fordav11]

Yes it's a lathe application.
its using G92. its a single thread cutting code. G92 does 1 cut then returns to the start position.

The normal type format is .....
G92 X10.0 Z-10.0 F12.7
X9.98
X9.96
X9.97
X9.95
etc

If the start Z is shifted slowly it can do a special thread profile with a single point tool.
For example....
G92 X10.0 Z-10.0 F12.7
G00 W-0.010
G92 X9.98 Z-10.0
G00 W-0.010
G92 X9.96 Z-10.0
G00 W-0.010
G92 X9.94 Z-10.0

etc

This is standard Fanuc G-code available on every controller from 3000C/6T to the very latest controls. Nothing special there.

This is a very simple example but to work this out properly for a real thread profile is not trivial. The amount of cuts required to cut a special form thread can easily run to 200+ but the control this gives a CNC programmer is amazing. *Any* thread profile can be done.

That's why I asked if Mastercam can do it.. Looks like not?

[WallyL7]

So I take it you are threading with a DNMG insert? (that is a new one on me)

And you also are using the same tool cycle to control the thread relief? (also a new one on me)....


If that is the case, then I am not sure mastercam will do it.

When threading on a lathe, though, most lathes respond to your incremental move by instead simply changing the starting position in absolute

your reference plane can be Z10. for the first threading cycle
then you can make it Z9.99 for your second pass. This starts the thread .010 closer to the part and removes material accordingly.

G0X10.Z10.
G92 X.000Z.000 R10. FXXX ETC
G0X10.Z9.99
G92 X.000Z.000 R9.99 FXXX ETC


I would say though that if you are just using your threading tool to control the relief, then use another toolpath to do that then thread normally.

Can you post the program you would use to do a complex type of thread and also a screenshot of what it looks like? I think I may be able to answer better that way.

[fordav11]

Check the attached sketch for an idea. If Mastercam can do this type of thread program generation it should be immediately obvious.

With reference to the sketch what I'm asking is if Mastercam can auto-generate a special thread given the angle of the sides (angles A and B), the depth (D) and a radius at the bottom (R). all of the cuts are generated long hand so also given is the tool nose radius which is used to calculate tool nose radius compensation.

I can't post the full program due to copyright.
Most threads in the oil and gas and mining industries are special threads.
It may be new to you but it's been going on for at least 30 years. Maybe more. That also suggests that Mastercam does not do special threads

[WallyL7]

New to me...lol Well, I am not going to say I've seen it all, but there isn't much that I can't figure out and now that I see a sketch, it looks quite simple. Your description was throwing me off at first.

Have you taken this to emastercam and asked? If I had to guess, I'd say Mastercam doesn't have a utility for that, but I would advise to check over there with those guys.

The "new" part for me was you using a canned cycle to cut the thread relief - which I now see you are not.

Funny how you make it seem so advanced and secret - but when I look at that it isn't. simple 2 axis lathe threads done with multiple start points and multiple diameters...it is that simple.

Have you even called mastercam to ask? (I know - it sounds kind of weird to actually call the company you have questions about...)

[fordav11]

well as I mentioned right at the start I did contact them some years ago and they didn't do it. I checked MCX4 and that doesn't do it either. I was hoping there would have been some recent advancements in that area with the latest version. Obviously not. I was also hoping to get a concise answer from a Mastercam expert.
it might be simple in theory but its not trivial to create this kind of CNC threading program.... there's also calculated tool nose radius compensation on every cut.
its basically a modified buttress thread. no secrets there.
However most of the info is tied up with patents and intellectual property rights
so the specific details and actual numbers *are* secret
I will have a look at emastercam.com thanks

[ak762]

so the specific details and actual numbers *are* secret

Do not make secret from unhidden
I believe such lathe functionality in Mastercam are welcome with great demand

[txcncman]

Question: Why are you using G92 instead of G76 for your threading?

[fordav11]

because each cut is separate. you cant control the tool start position on every cut using G76.
G76 is for cutting standard threads using regular form inserts or even special form inserts. but the insert shape controls the final profile of the thread whereas using the G92 method a single point tool can cut any profile.... much like the pics above.

[fordav11]

hmmm that's an interestingly small picture....to hide secret details
what program is that?

[ak762]

It is just NC code
If I recall right it was generated by FeatureCAM by clever doc one
and verified in NCManager

[fordav11]

ah G32. I use that on a Mazak Multiplex because it doesn't accept G92. But it does the same thing

[txcncman]

Why do you need to control tool start position? Isn't the DNMG insert just cutting its own profile? Are you trying to control amount of engagement?

With G76 you can have some control of engagement with the P word.

Pxxyyzz - where xx = repetitions (normally set to 01)
yy = chamfering amount (normally set to 00)
zz = angle of tool tip (only 80, 60, 55, 30, 29, and 00 allowed
normally set to 60 for standard "V" thread)

[fordav11]

I know about G76, it's not useful in this case. Check the large pic above showing code (its using G32 instead). You can't get that kind of tool control with G76.
Anyway, I got my answer, Mastercam does not do what I want so this thread is complete. And so is the thread

[ak762]

I know about G76, it's not useful in this case. Mastercam does not do what I want so this thread is complete. And so is the thread

fordav11, open your mind
I think Mastercam can not do it in one click at this moment. But with additional actions I am sure you can achieve appropriate result.
I would look into surface strategies ( generate start points from profile with flowline op. with suitable scallop height )

[fordav11]

I'm waiting for the 1 click solution. maybe 3 clicks tops but no more!
actually my knowledge of Mastercam doesn't really extend past 2.5D mill work and turn/mill lathe work with C/Y so I'll have to wait for an easier option and do it my long-hand way in the meantime
I see there's a trial version of Feature Cam available so I'll check that out.

[WBODDE]

Looking to buy MC X current version. Just wondering if Mastercam can generate special threads using a single point tool? For example a thread with 20 degrees front angle and 45 degrees back angle with a 0.1" rad at the bottom by 0.25" deep using a common PDPNN tool with DNMG insert and multiple G92 lines? I remember inquiring directly to Mastercam a few years back (around when MC X was released) and they said it was planned but not a priority. I don't need anything else from any CAM software except this. The rest I can do on the machine
We do it now using Autocad and manually work out the cuts but it's a PITA
Is there any better solution (or any solution?) for auto-generating special threads?

have not found one yet out thread but know what you are talking about but did my contour with a custom macro on my cheap power station setup to just put line vert the step over amount.then when my program pick each end of line and let it post it out. worked great on a convec/concave round thread using what ever tool nose rad on insert
.

[ERUS]

Mike is right. All the lathe is doing is running at the feed per revolution for whatever pitch of thread you're cutting.

The thread profile is entirely based on the tool geometry.

I cut a wood thread with a 0.078" cutoff tool and a regular 60 degree threader. The threader insert cut the sharp angle at the outside of the thread and the 0.078 groover actually cut the majority of material out. Get my offsets timed was a pain, but it works and is repeatable.