What's new
What's new

Seeking help for manufacturing multi-start acme threads via thread mill

oilpig

Plastic
Joined
Jul 22, 2016
Hi, guys. I am trying to machine multi-start acme threads by using thread mill and HAAS VF-0E. I am using a small thread mill from INTERNALTOOL, shown as follows,
threadmill.jpg
The two-start acme thread looks not bad (OD=6.594mm, ID=4.498mm),
2start.jpg
However, the four-start acme thread looks bad, most part of the crest of the thread has been removed (OD=6.594mm, ID=4.498mm),
4start.jpg

Can anyone give some suggestions to solve this problem? Thank you!
 
it looks like the pitch of your thread is too great for the tool to cut it. as it steeply pitches the cut it cuts away previous threads. you need a different tool/setup.
 
Threadmill cannot make a correct threadform when the helix angle is too great (without adding another axis). In fact, I rather doubt your 2-start thread is correct either.

This can be correctly done at the lathe with a single-point tool (held at a sufficient angle), or at the mill with a 4th axis and a tapered EM.

Regards.

Mike
 
Thank you! I am using the tool for 1.6 mm pitch, which is the same as the pitch of my design.
 
Threadmill cannot make a correct threadform when the helix angle is too great (without adding another axis). In fact, I rather doubt your 2-start thread is correct either.

This can be correctly done at the lathe with a single-point tool (held at a sufficient angle), or at the mill with a 4th axis and a tapered EM.

Regards.

Mike

Hi Mike,

Thank you! Is there any referenced material for writing a G-CODE for multi-threads with a 4th axis? What do you mean by tapered EM? Do I need to order another tapered endmill?

Best,

Aoyu
 
You can cut square threads first with a groove tool, then taper down each side 14.5 degrees, if your machine has a cycle for that.
It's been a few years so I don't remember the codes, but I did it on an Okuma.
 
You can cut square threads first with a groove tool, then taper down each side 14.5 degrees, if your machine has a cycle for that.
It's been a few years so I don't remember the codes, but I did it on an Okuma.

Thank you very much!
 
Hi oilpig:
As Finegrain has pointed out, you cannot cut a coarse pitch small diameter Acme thread on a VMC with a threadmill; the helix angle of the thread is so steep that the profile of the thread gets boogered by the threadmill.
You need to be able to tilt the threadmill so its axis is at right angles to the helix, and only a thread milling machine, a mill turn or a 5 axis mill can do that easily.
It is possible to stand up a 4th axis on the helix angle and program a cutter path that follows the slope of the 4th's axis, but it's a real pain to do it that way.
Alternatively as Finegrain suggests, you can get a tiny endmill that has the proper shape to cut the thread profile and end mill it in with the part held horizontally in the 4th.
Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
www.vancouverwireedm.com
Clarus Microtech Inc. | Facebook
 
Hi oilpig:
As Finegrain has pointed out, you cannot cut a coarse pitch small diameter Acme thread on a VMC with a threadmill; the helix angle of the thread is so steep that the profile of the thread gets boogered by the threadmill.
You need to be able to tilt the threadmill so its axis is at right angles to the helix, and only a thread milling machine, a mill turn or a 5 axis mill can do that easily.
It is possible to stand up a 4th axis on the helix angle and program a cutter path that follows the slope of the 4th's axis, but it's a real pain to do it that way.
Alternatively as Finegrain suggests, you can get a tiny endmill that has the proper shape to cut the thread profile and end mill it in with the part held horizontally in the 4th.
Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
www.vancouverwireedm.com
Clarus Microtech Inc. | Facebook

Thank you for your summary! However, what do you mean by a thread mill machine or a mill turn? What is the difference between a thread mill machine and a traditional mill? What is the difference between a mill turn and a lathe?
 
Hi oilpig:
A millturn machine is basically a glorified lathe that has a milling head which can be articulated to present a cutter at any angle to your workpiece.
A very popular model is Mazak Integrex, but there are many others you could Google if you want more details.
The ability to tilt the head and drive it in X,Y and Z is what makes it different from a normal live tooled lathe, and the fact you can turn with it and bar feed it differentiates it from a 5 axis mill.
If you run insert cutters on your milling machine, the cutter bodies were likely made on a millturn.

A thread milling machine is a specialist machine who's sole purpose is to machine threads (usually on parts like machine leadscrews), hob profiles and worm profiles, and the general layout is like a cylindrical grinder.
It uses a custom profiled saw that can be tilted to the helix angle of the thread to mill the gullets.
Often these are then finished on a thread grinder which is laid out basically the same but substitutes a big formed grinding wheel for the milling cutter.
The ability to tilt the wheel and the ability to gear the rotation of the workpiece to the Z axis traverse (just like an engine lathe) is what distinguishes these machines.

Cheers
Marcus
Implant Mechanix • Design & Innovation > HOME
www.vancouverwireedm.com
Clarus Microtech Inc. | Facebook
 
Hi oilpig:
A millturn machine is basically a glorified lathe that has a milling head which can be articulated to present a cutter at any angle to your workpiece.
A very popular model is Mazak Integrex, but there are many others you could Google if you want more details.
The ability to tilt the head and drive it in X,Y and Z is what makes it different from a normal live tooled lathe, and the fact you can turn with it and bar feed it differentiates it from a 5 axis mill.
If you run insert cutters on your milling machine, the cutter bodies were likely made on a millturn.

A thread milling machine is a specialist machine who's sole purpose is to machine threads (usually on parts like machine leadscrews), hob profiles and worm profiles, and the general layout is like a cylindrical grinder.
It uses a custom profiled saw that can be tilted to the helix angle of the thread to mill the gullets.
Often these are then finished on a thread grinder which is laid out basically the same but substitutes a big formed grinding wheel for the milling cutter.
The ability to tilt the wheel and the ability to gear the rotation of the workpiece to the Z axis traverse (just like an engine lathe) is what distinguishes these machines.

Cheers
Marcus
Implant Mechanix • Design & Innovation > HOME
www.vancouverwireedm.com
Clarus Microtech Inc. | Facebook

Thank you very much! However, I still cannot imagine how to use 5-axis mill to machine multi-start threads. I am going to describe my question as follows,
threadmill-5axis.jpg
As the left portion of image shown, it is ok if I tilt the working piece(material in the image) to a specific angle for machining initial threads. However, I cannot machine the remaining threads away from the top of the working piece, because it will cause collision to the thread mill and the working piece, as the right portion of the image shown. Can you give me some suggestions?
 
Why would u have the material tilted toward the cutter? The problem is the helix angle is to great on acme threads, so trailing end of the cutter cuts into the part where it shouldn't. What needs to be done on a 5 axis is keep the tool tangent to the material while tilting the tool toward the helix angle.

Also in the previous post about a tapered endmill and a 4th axis, he means holding the material along the X or y axis and milling the thread (OD only) with a tapered endmill the same angle/form as the thread. Basically single point threading but in a mill instead of lathe.
 
What some of the guys are trying to explain about the 4th axis is similar to my pic.

Mine was just a square 4 start thread so you would need a cutter with the correct profile for your thread. Even then I would probably rough it out with a square tool and just use the profile cutter for finishing up.
 

Attachments

  • DSC_0594.jpg
    DSC_0594.jpg
    90.4 KB · Views: 1,865
Why would u have the material tilted toward the cutter? The problem is the helix angle is to great on acme threads, so trailing end of the cutter cuts into the part where it shouldn't. What needs to be done on a 5 axis is keep the tool tangent to the material while tilting the tool toward the helix angle.

Also in the previous post about a tapered endmill and a 4th axis, he means holding the material along the X or y axis and milling the thread (OD only) with a tapered endmill the same angle/form as the thread. Basically single point threading but in a mill instead of lathe.

Thank you! you unlock my confusions!
 
What some of the guys are trying to explain about the 4th axis is similar to my pic.

Mine was just a square 4 start thread so you would need a cutter with the correct profile for your thread. Even then I would probably rough it out with a square tool and just use the profile cutter for finishing up.

Thank you for intuitive perception!
 








 
Back
Top