PDA

View Full Version : Need Help! Cutting internal threads inside large acrylic tubes.



cvriv.charles
03-02-2009, 10:47 AM
Hi. I was wondering how one would go about cutting internal threads for acrylic tubes with internal diameter's varying from 1.75 - 2.25"?

An example:
http://www.performance-pcs.com/catalog/images/products/15700_01.jpg

I was thing a lathe. I saw a guy cutting external threads for a steel rod using a lathe by constantly starting and stopping the machine going back and forsth with the drive system. I thought that maybe I could do that. That would be very hard though because I only want to thread in about a 5/8". Would be hard determining when to stop the lathe. Plus,... I would have to turn the lathe slow to make it easier to stop at a certain point inside the tube. Acrylic doesnt really cut all that well at really slow speeds.

I was thinking about converting a manual lathe into cnc lathe but im sure that would be very painful seeing that the bit would have to know exactly the chuck is on it's rotation plane to make several passes to cut the treads.

Then I though that make there was a huge special tap out there somewhere? But im sure that would be a pain too.

What about using a mill or a router to cut the threads with the tubes mounted vertically with some special horizontal vgrooving bit?!?!? I dont know.

Any help/ suggestions would be great. Thanks.

Geof
03-02-2009, 10:55 AM
Huge special tap is out for acrylic, it would almost certainly shatter.

If you are dealing with extruded acrylic forget it, it will stress crack almost immediately; you must use CAST acrylic.

If you have a CNC mill that is capable of helical interpolation you can thread mill. This could be a preferred method because the cutting load is low.

If you do attempt it in a lathe hold the acrylic tube inside a closely fitting split sleeve made out of aluminum and nicely polished inside so it will not mar the acrylic.

Acrylic machines, or thread, okay at low speed but your tools have to be ultra-sharp, carbide insert threading tools are not suitable you should grind your own in HSS; remember zero top rake for acrylic.

Dentedcrown
03-02-2009, 10:59 AM
I needed to do something similar once to a piece of palstic. I got a pipe nipple from the hardware store and cut slots with my chop saw through the threads. Made a makeshift tap that worked pretty well with the plastic. Might work with acrylic...

DC

cvriv.charles
03-02-2009, 04:30 PM
What is required of a cnc mill to cut internal threads? Helical interpolation? What is that?

Geof
03-02-2009, 05:04 PM
What is required of a cnc mill to cut internal threads? Helical interpolation? What is that?

Creating a helical path. CNC mills can do circular interpolation clockwise using the G02 command or counterclockwise using the G03. When the machine can combine motion of the Z axis in synchrony with the circular interpolation then the path of the cutter is a helix. If the cutter is a threading tool the machine generates a thread.

Al_The_Man
03-02-2009, 05:17 PM
I was thinking about converting a manual lathe into cnc lathe but im sure that would be very painful seeing that the bit would have to know exactly the chuck is on it's rotation plane to make several passes to cut the treads.
.

Actually CNC takes the pain out, as the control system synchronizes the tool with the spindle, similar to described for helical milling.
I think your problem with a lathe, you need to obtain one with sufficient through hole and that dia generally means a large machine, which you do not necessarily need a great deal of power for that application, so you could end up with overkill on the power end of things.
Al.

cvriv.charles
03-02-2009, 07:08 PM
Creating a helical path. CNC mills can do circular interpolation clockwise using the G02 command or counterclockwise using the G03. When the machine can combine motion of the Z axis in synchrony with the circular interpolation then the path of the cutter is a helix. If the cutter is a threading tool the machine generates a thread.

Is it that much more complicated to make a cnc mill that can move all axis's at once?

Geof
03-02-2009, 08:07 PM
Is it that much more complicated to make a cnc mill that can move all axis's at once?

No, it is an operating software issue. I think on some machines the ability to do helical interpolation is an option. The machines I use, Haas, include it as a standard feature.

cvriv.charles
03-02-2009, 08:10 PM
No, it is an operating software issue. I think on some machines the ability to do helical interpolation is an option. The machines I use, Haas, include it as a standard feature.

I'm assuming I couldnt perform this type of task with a cnc router could I?

Geof
03-02-2009, 10:03 PM
I'm assuming I couldnt perform this type of task with a cnc router could I?

That is a good question. How much Z travel does your router have? To my knowledge most are quite short. Does your control do helical interpolation?

If you have the travel, if the control can perform the motion, then possibly.

It is only 'possibly' because routers go fast and probably you will find you get melting of the acrylic. When machining acrylic with a router you need very fast feed because if you go slow things get to hot. Very fast feed and helical interpolation don't go together very well.

cvriv.charles
03-03-2009, 01:42 AM
That is a good question. How much Z travel does your router have? To my knowledge most are quite short. Does your control do helical interpolation?

If you have the travel, if the control can perform the motion, then possibly.

It is only 'possibly' because routers go fast and probably you will find you get melting of the acrylic. When machining acrylic with a router you need very fast feed because if you go slow things get to hot. Very fast feed and helical interpolation don't go together very well.

Well,... I havent actually built my cnc router yet. I am trying to get an idea of all the different tasks I will be doing so that I can better build the machines I will be using.

My know for fact that my cnc router will not have a lot of z travel. I was thinking that the secret to using a cnc router to cut internal threads for these tubes would be the table itself. I would have the tube mounted in such a way that they would pass through the table hanging mostly under the table. If I could do that then the only other thing would be the melting problem. But that can be solved by adding a cooling system. A bit of water when cutting acrylic help a lot. I'm not worried about the melting really. It's the cutting bit itself. I'm not familiar with these bits. I dont know what their max operation speed is. I was thinking it would be something like and end mill which is usally used at much lower speeds then what router bits are used at. You know what I mean?

mc-motorsports
03-03-2009, 02:03 AM
Threadmilling is probably the way to go on that job. It would be more reliable than having to chuck or lathe fixture and spin the tube... And you could do single point threadmilling if your worried about the material cracking and what not. or inserted multi-point threadmilling would go much faster.

One shop I used to work at threadmilled ABS plastic parts because #1, it was something like a 2" NPT thread and #2 even if they had a machine that could run that tool, taps aren't very forgiving in plastics, they like to rip and chew.

Threadmills have a great place in manufacturing and can be used to solve many problems. Yet you do have the option of spinning that part in a lathe, I would still look into threadmilling.

cvriv.charles
03-03-2009, 02:07 AM
Threadmilling is probably the way to go on that job. It would be more reliable than having to chuck or lathe fixture and spin the tube... And you could do single point threadmilling if your worried about the material cracking and what not. or inserted multi-point threadmilling would go much faster.

One shop I used to work at threadmilled ABS plastic parts because #1, it was something like a 2" NPT thread and #2 even if they had a machine that could run that tool, taps aren't very forgiving in plastics, they like to rip and chew.

Threadmills have a great place in manufacturing and can be used to solve many problems. Yet you do have the option of spinning that part in a lathe, I would still look into threadmilling.

Yea im thinking threadmilling is the way to go. I really would like to get a router to do the job. I have to do some research on the threadmilling bit.

Al_The_Man
03-03-2009, 10:54 AM
The only problem I can see is using the high rpm spindle motor that a router uses, especially if Universal Motor type.
I think you may have to fit a custom spindle motor for high torque at low rpm.
Al.