What's new
What's new

Thread turning with a grooving tool

Joined
Nov 21, 2023
Hello.
I am looking for software to generate acme threads on a lathe using a tool to 'work' its way down the slope of the thread.
I have had someone generate code for me in the past like this, but I am unable to get it made by them any more.
Basically I use a grooving type tool (small corner rad .008) and the code cuts down the slope of the thread form a few thousands at a time, moving the Z back and forth each subsequent pass
to form the thread shape. It steps down and back/forth each pass. The tip width of the grooving insert is smaller than the root width of the thread.
This type of code works really well because you can adjust the width of the thread form using the tool offsets. It is quite easy to produce a high quality thread.
We use this type of program when we are doing stainless materials or multi-start threads. These scenarios are more difficult with a full profile tool due to the large surface contact when the tool is near full depth.
The other nice thing with being able to produce code to do this is that you can make any shape of 'thread' that you want.

Anyhow, to summarize (TL;DR) I am looking for software that will generate code to turn acme threads on a lathe using a grooving tool.

Thanks
 
Hi Wyrks Tool & Machine:
You may have some problems finding off-the-shelf software to do this easily.
Two problems I'm aware of:
1) Some turning software will not permit doing operations with a tool that has been defined for a different function.
I'm reasonably familiar with two...HSMWorks and Mastercam.
If you take a stock grooving tool from the Mastercam tool library for example, it won't permit anything other than grooving and parting...you get some dumb message that says "No you can't do this"
So you have to create a custom tool, making a solid model of the insert and defining it as a threading tool.
Same insert shape, same holder, but defined differently in the software.

2) Setting up the threading cycle is complicated...you need to write several separate toolpaths and then combine them:
One to get into the part to full depth.
One to widen the root of the thread.
One to shave the trailing flank incrementally
One to shave the leading flank incrementally.
You jigger the start point of each cycle to get the width correct.

It's probably easiest to just post them as separate operations and then eliminate the redundant bits by hand.
As I say, my familiarity with Mastercam (what I'm using now) is still pretty weak( four months experience), but that's where I would start.
I can do each of the cycles I described...no reason I can see that I can't just run them one after the other when I post them.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
 
Last edited:
Mastercam Lathe has a Custom Thread toolpath that does stuff like this but it has limitations.
That looks like what I need. The one that the guy used in the past for me was his own program (won't sell me a copy, I have asked many times) and it was very similar to that. You would enter all of the thread data, your parameters and your tool shape and it would generate G-code to generate the thread.
Unfortunately I don't have Mastercam so I am hoping to find a stand-alone, or cheaper option.
Thanks for the reply.
 
Hi Wyrks Tool & Machine:
You may have some problems finding off-the-shelf software to do this easily.
Two problems I'm aware of:
1) Some turning software will not permit doing operations with a tool that has been defined for a different function.
I'm reasonably familiar with two...HSMWorks and Mastercam.
If you take a stock grooving tool from the Mastercam tool library for example, it won't permit anything other than grooving and parting...you get some dumb message that says "No you can't do this"
So you have to create a custom tool, making a solid model of the insert and defining it as a threading tool.
Same insert shape, same holder, but defined differently in the software.

2) Setting up the threading cycle is complicated...you need to write several separate toolpaths and then combine them:
One to get into the part to full depth.
One to widen the root of the thread.
One to shave the trailing flank incrementally
One to shave the leading flank incrementally.
You jigger the start point of each cycle to get the width correct.

It's probably easiest to just post them as separate operations and then eliminate the redundant bits by hand.
As I say, my familiarity with Mastercam (what I'm using now) is still pretty weak, but that's where I would start.
I can do each of the cycles I described...no reason I can see that I can't just run them one after the other when I post them.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
Yes, I could manually write the code, but I make a few different threads, internal and external, and I was hoping to find a turn-key solution.
Thanks for the reply.
 
Hi Mtndew:
Yet again, you've taught me something new...I had no idea this option exists.
I owe you big time by now for all the things you've revealed on here about how to work the software.

I've gotten as much from you in just these postings over the years than I got when I participated in the Mastercam training that came with my purchase of the software.
This is not a slur on the trainer, but he had a lot to cover and I'm an old fart...resistant to learning new technology, by virtue of my ossified brain cells.

So thanks for that (yet again).

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
 
Featurecam can do this no problem if you know anyone who has it and a compatible post.

I have FC, but no posts for either of your machines.

Edit: Actually, you might be one of the extremely rare "good candidates" for the autodesk's subscription service...
 
Good morning everyone. I just wanted to post a follow up on this thread.

I contacted https://www.buntetec.de/software/cnc-gewinde for the thread program that he offered. He was good to work with and he was able to make an English version of the software for me. Unfortunately his program will only generate code in Metric output, not Imperial (inch). 99% of the threading we do is Imperial so this was something that I couldn't use practically. I realize that I could convert all my data to Metric and put the lathe in Metric mode, but my guys are Imperial minded and I think this would lead to more problems thereby making it not practical for us.
If you do Metric threading and need something like this I would recommend looking at this software. It seemed quite easy to use.
 
If you were to draw the shape of the thread profile in any cad system then just figure out where your tool contacts this profile on each cut. Then just use a sub program to run a g32 threading cycle at each one of the starting points. After it makes a cut have it go back to the main program to get the next starting point and run the sub program again. Keep doing this until the whole thread is cut.
 
If you just find your start points and run a program with a sub like this
 

Attachments

  • PXL_20231211_160952891.jpg
    PXL_20231211_160952891.jpg
    4.5 MB · Views: 4
Last edited:
If you just find you start points and run a program with a sub like this
It's a fine idea in principle, but in practice that would be a lot of work for a typical continuous profiled thread - the number of passes is usually huge compared to a typical threading cycle.

If you just had to do it once, or maybe twice, this would be a fair suggestion.

More often than that and anyone who values their time (or sanity) is going to want to find a better way.

Like I said earlier, Featurecam has had this functionality for as long as I can remember, and I have used it many times over the years to make some enormous threads, custom threadforms, rope drums etc.
 
If you had a program that would do it, that would be great. The way I showed, the only thing that takes time is finding the start points. My old bobcad program spits the code out in seconds.
 








 
Back
Top