Sorry, I didn't read the thread as carefully as I should have. Nice lathe you got there btw!

 

PVC won’t “chip”. It’s the nature of the material. I’ve always got those long strips of material. And a spiral fluted drill bit will probably still give you trouble, because once the string is pulled out of the hole, it will wrap around the drill shaft and chuck. Perhaps a chemist or materials engineer can explain why. I’ve used PVC a lot in the day, making skeletons for Halloween monsters.

 

PVC won’t “chip”. It’s the nature of the material. I’ve always got those long strips of material. And a spiral fluted drill bit will probably still give you trouble, because once the string is pulled out of the hole, it will wrap around the drill shaft and chuck. Perhaps a chemist or materials engineer can explain why. I’ve used PVC a lot in the day, making skeletons for Halloween monsters.

Ok... thanks for sharing... I know it won't "chip" but it does "flake" when it's routed.

any ideas?

 

I've used them on sheet plastic (also PVC), and they work fine too. But most likely their usefulness is limited to thin types of material.

Not so! See my post about this exact thing. I got a wild hair and decided to try boring a 1.5" hole through 3" of steel with a cheap Amazon straight-fluted step drill and it worked like a charm. Unbelievable. I've been doing ever since, never an issue.

You can get them with spiral flute also.

Yes you can, and they are excellent. I've put all my old cheap and/or non-fluted step drills in box that I reach into when someone asks to borrow, and what I use exclusively nowdays are these.

So excellent. They drill panel holes in a fraction of the time, taking a real bite of metal every revolution instead of little slivers and splinters. They make chips 1/8" thick that make "ting" sound when they hit the ground and you can't even bend them by hand. I've only managed to damage one of them and I'm not even sure I did it myself; I think one of my ham-fisted coworkers may have borrowed it without asking to do something predictably stupid like open up a hole in a railroad track at 5,000rpm. It has chips knocked off the steps at 1/2" so I just use it for larger holes now.

Strantor, I finally got myself a lathe ... in fact, I bought one of these. ... eat your heart out!

Dude! I've spent probably a cumulative week starting at pictures of that. I am (currently) concurrently designing and building a special purpose little CNC machine based loosely on that Taig/Sherline CNC concept (gang tooling on a stupidly long cross slide). It will be a Swiss lathe. I struggled with whether to buy that Taig/Sherline and modify it to suit my needs or build from scratch, and ultimately decided to build from scratch as there would be so much modification that only the headstock would remain unmolested. So I bought the Sherline headstock and collet closer which I'll automate to interface with a bar feeder. Rev0 will be the headstock mounted horizontally to my CNC mill column and using the mill's table as the cross slide with gang tooling bolted down to it. But anyway enough about that, super cool, I'm happy for you.

After careful consideration, my conclusion is that the problem is that the material is being cut into long strips, instead of being chipped. And those strips have no way out of the bore being drilled.

Yes, I agree with your conclusion. This is a common challenge drilling/boring plastics. One thing you could try if the strings aren't making their way out of the cut, is plan your progressive up-sizing of bits such that your final pass bit is only taking off a little, leaving enough room for the strings to accumulate in the flutes with getting absolutely crammed in so tight that they're rubbing and friction-ing and melting against the walls of the hole. But you can't cut it too close, because (may not apply to PVC) if there isn't sufficient difference between [this] drill and [last] drill, the bit might not actually cut the plastic, but instead just push it, deform it outwards, stretch it, and make a whole lot of undesirable friction and melty-ness in the process.

Also important that you use a very sharp bit with appropriate point, cutting, and relief angles for plastics. Your hardware store's 135 degree general purpose black oxide bit might not be the right tool for the job. Check out these drill bits for plastics; look a bit odd don't they?

I've been cutting solid PVC using a CNC router for many years now, and it's never been a problem. Using an end mill at high speed produces many light chips resembling flakes that are easily pulled up and blown out of the way by the spindle itself.

I know it won't "chip" but it does "flake" when it's routed.

any ideas?

When you talk about the different results from your CNC router are you talking about milling or drilling? I assume milling. Keep in mind that they're totally different. Milling is a perpetual interrupted cut and drilling is... drilling. Your end mill is making those same strings but they're only produced on the leading edge of the end mill and then the flute is out of the cut, coming around the back side, and the "chip/flake" is expelled as if it had been sliced off by a rotatating knife, because it was, and then the next flute comes into the cut and does the same thing. Hence the nice clean flakes. But a drill bit is going straight in, uninterrupted cut, so that produces one long string. If you were to somehow "unwrap" that hole and turn it into a straight line, this is what's happening when you're milling:

And this is what's happening when you're drilling:

Maybe the easiest option with the tools you already have, is mill the hole out on your CNC with a helical pattern.

 

I've been cutting solid PVC using a CNC router for many years

Not knowing how deep this hole is or needs to be, if you have a CNC router, why not just use it? One of the things that many if not most machine shops the have CNC now days do is program big holes and rout them instead of using a boring head to do it. Just get a long end mill and go for it.

 

Not knowing how deep this hole is or needs to be, if you have a CNC router, why not just use it? One of the things that many if not most machine shops the have CNC now days do is program big holes and rout them instead of using a boring head to do it. Just get a long end mill and go for it.

The bore is 35mm in diameter, and 95 mm long. And my router can handle cutters of up to 10mm in diameter. I'm not aware of any cutter of that diameter that is long enough to do the job.

On the other hand... plan B would be to first route the bore from one side, and then turn the part around and bore it from the other side.... I'm gonna have to think about it some more

 

The bore is 35mm in diameter, and 95 mm long. And my router can handle cutters of up to 10mm in diameter. I'm not aware of any cutter of that diameter that is long enough to do the job.

On the other hand... plan B would be to first route the bore from one side, and then turn the part around and bore it from the other side.... I'm gonna have to think about it some more

"YG-1 - 55901 E5065 Carbide Square Nose End Mill, Extra Long Reach, Uncoated (Bright) Finish, 30 Deg Helix, 4 Flutes, 6" Overall Length, 0.25" Cutting Diameter, 0.25" Shank Diameter: Amazon.com: Industrial & Scientific" https://www.amazon.com/YG-1-Carbide...ocphy=9061125&hvtargid=pla-662183794773&psc=1

 

"YG-1 - 55901 E5065 Carbide Square Nose End Mill, Extra Long Reach, Uncoated (Bright) Finish, 30 Deg Helix, 4 Flutes, 6" Overall Length, 0.25" Cutting Diameter, 0.25" Shank Diameter: Amazon.com: Industrial & Scientific" https://www.amazon.com/YG-1-Carbide...ocphy=9061125&hvtargid=pla-662183794773&psc=1

Nice! ... but it has a cutting length (flute length) of only 1-1/2" inches... And I need 3-3/4", or 2" at the very least.

 

"YG-1 - 55901 E5065 Carbide Square Nose End Mill, Extra Long Reach, Uncoated (Bright) Finish, 30 Deg Helix, 4 Flutes, 6" Overall Length, 0.25" Cutting Diameter, 0.25" Shank Diameter: Amazon.com: Industrial & Scientific" https://www.amazon.com/YG-1-Carbide...ocphy=9061125&hvtargid=pla-662183794773&psc=1

With most hobby CNC machines and the Taig type lathe I would neve attempt to use carbide tooling. The spindles don't have near enough power and the whole machine lacks the rigidity to get the benifits of the carbide. Plus HSS is much sharper. But then again I only did this machining stuff since I was 17 years old so what do I know.

 

The spindles don't have near enough power and the whole machine lacks the rigidity to get the benifits of the carbide.

I don't know about the rigidity thing (as far as my problem goes... but I bet you're most probably right), but the spindle does have enough power... the problem with it is that the way it's designed, the motor is hinged on its own weight and the belt tends to slip easily. I've had to push it down to tighten it a bit while it's at work to prevent that from happening sometimes.

 

With most hobby CNC machines and the Taig type lathe I would neve attempt to use carbide tooling. The spindles don't have near enough power and the whole machine lacks the rigidity to get the benifits of the carbide. Plus HSS is much sharper. But then again I only did this machining stuff since I was 17 years old so what do I know.

Was that preemptive defensive sarcasm or do you feel that I've already challenged your expertise? If I did, I didn't mean to. We've shared this space for years and I know enough about you to formally and publicly acknowledge that you are the more experienced by a huge margin.

Anyway, I was suggesting that to be used on his CNC router, not on the taig lathe.

 

Nice! ... but it has a cutting length (flute length) of only 1-1/2" inches... And I need 3-3/4", or 2" at the very least.

Why? You could take incremental circular passes. If you're worried about the unfluted portion of the tool shank contacting the wall of the bore on the deeper passes, I don't see the problem, but if it is one, you could get a reduced shank XL endmill so that the unfluted shank will not touch the wall.

 

If you're worried about the unfluted portion of the tool shank contacting the wall of the bore on the deeper passes, I don't see the problem

Unfortunately, it is a problem. I've tried already with other different PVC parts and when the solid portion of the shank brushes against the already cut part (because the cutting part of the tool has the exact same diameter) the material heats up and leaves an unacceptable rough finish.

But I didn't know about reduced shanks XL endmills... thanks for the tip, I'm gonna look it up.

 

Unfortunately, it is a problem. I've tried already with other different PVC parts and when the solid portion of the shank brushes against the already cut part (because the cutting part of the tool has the exact same diameter) the material heats up and leaves an unacceptable rough finish.

Good to know, I've never tried this so if I ever do, I'll already know what I'm walking into.

 

But I didn't know about reduced shanks XL endmills... thanks for the tip, I'm gonna look it up.

Not cheap but maybe you can find something else on the website that would work for you and not break the bank

https://www.harveytool.com/products/tool-details-943228



Anyway that's just an example. I'm sure you could find cheaper if you invest time in looking.

 

Not cheap but maybe you can find something else on the website that would work for you and not break the bank

https://www.harveytool.com/products/tool-details-943228

View attachment 237960

Anyway that's just an example. I'm sure you could find cheaper if you invest time in looking.

Interesting... they're calling a 6" long, 3/8" dia end mill a "miniature" !

 

I may have missed what the goal is but one solution that comes to mind is to find a PVC pipe of the right ID and insert it into your rough hole drilled to the OD of that pipe. The PVC adhesives are very good. It would truly be one piece.

 

Was that preemptive defensive sarcasm or do you feel that I've already challenged your expertise? If I did, I didn't mean to. We've shared this space for years and I know enough about you to formally and publicly acknowledge that you are the more experienced by a huge margin.

Anyway, I was suggesting that to be used on his CNC router, not on the taig lathe.

NO please don't think that! I have great respect for you and have tried to help anyway I can. But many here dismiss my suggestions when it comes to machining. And some others that claimed to be friends turned out not to be. They know what I mean. What I know works comes from many people sharing things with me and my own experiences. Much of what is in books on machining and even taught in say trade schools is based on books and ideas that are way out dated or only work in perfect situations. Kind of like how the perfect capacitor or IC doesn't exist when using LTSpice or other design programs perfect machining doesn't exist in the real world either.

For what is being done here a hobby CNC mill or Taig lathe isn't or wouldn't be my go to machine. They are toys, meant for making other toys, not doing real work. The ~$4K to buy a taig to me would have been better spent on a real lathe and some tooling. The small table top machines are fine for making simple small non critical parts, but when it comes down to holding tolerances and repeatability nothing beats mass of the machine it's self.

 

Ok, here's what worked in the end:

Using my lathe, I was able to (very slowly) drill through the part using a step drill bit with a maximum diameter of 32mm, exactly like this one:

​

What I did was make a program that would drill the hole by pecking it in increments of 1mm at 450 rpm while blowing the plastic threads away using an air gun. It takes quite a while to do it that way, but it gets the job done and leaves an acceptable rough surface finish.

I then made a boring bar made out of a 1" diameter rod, and installed a high speed steel cutting tool on its tip. The tool's cutting diameter can be adjusted by turning a #4-40 set screw:

​

This tool left a spectacular surface finish, and it enlarged the 32mm bore to a diameter of 35mm on a single pass at 800 rpm and a feeding speed of 60mm/min.

My conclusion is that I should get myself either a bench drill or a milling machine to make the preliminary 32mm bore using traditional drill bits, and finish it on my lathe using the boring bar. This because drilling it using my lathe as a drill proved to be too cumbersome.

 

This tool left a spectacular surface finish, and it enlarged the 32mm bore to a diameter of 35mm on a single pass

See my telling you to remove it with a heavy finish pass works. If you have a mill with enough quill travel why not just get a boring head for it? After you use one you will find more and more uses. You then no longer need to have a large number of drills and you can even make holes in between standard sizes.