Deep narrow irregular holes in plastic: what bit?

[jonboycnc]

Hi everyone,

I need to cut irregularly shaped holes in plastic (probably polyethylene or flexible PVC).

Because they need to be very small and precise, I'm planning to buy as benchtop cnc mill.

The nasty thing is that these irregularly shaped holes need to be 1 cm (1/3 inch) (ideally even 2cm) deep but sometimes as narrow in places as 0.5mm (a little more than 1/64 inch).

What kind of cutting bit could do this, and how?

I've seen drill bits this narrow, and I don't mind using an approach of drilling many contigous small holes instead of sideways routing. But I worry that because drill bits are conical at the tip, if the holes overlap too much the tiny drill bit will bend into the existing hole rather than cutting a new one.

I'm totally new to the world of cutting bits and CNC. If I knew the right terminology I could google more on what sizes were available, but I don't ...

Tiny, deep, cutting bits anyone???

Thanks!

Jonathan

[Jeff-Birt]

I would suggest starting by looking at the machinability of the materials you mentioned. Plastics can be really hard to machine as they can get soft and gummy and will expand as they heat up.

If your stuck ,give me a call and I'll see if I can help you find the proper bits. My contact info is on my website.

[jonboycnc]

Thanks for the reply Jeff - really appreciated.

The parts I'm machining have to be cast/molded, hence why the thermoplastics. I could move to Nylon (much higher melting point) fairly easily if I couldn't get polyethylene or pvc to work.

Moving away from thermoplastics to resin, plaster or white metal would be a hassle, though not impossible if absolutely necessary.

Those PreciseBits deep reach end mills you carry look like the kind of thing I might need to get into, if simple drill bits are not good enough.

[One of Many]

Chances are very slim you will find cutters that small with cutting lengths that long. It may be just as hard to locate short cut lengths with extended shanks. Either case, they won't be cheap if rare.

Poly base plastics being soft do not take well to making small chips either, which leads to heat and melting in short order at spindle speeds required for smaller cutters. Good luck getting chips out of the way. Dunno if one of them vortex generating air coolers would help here.

If these are through holes or the bottom depth of cutout were not all that critical, you might consider a custom broach possibly even heated to leave the shavings in the bottom of the hole compressed or clear through for deburring.

That's a tough one, but if there's a will....!

DC

[TDA]

Drills and end-mills both have advantages and disadvantages for this application. Unfortunately neither is probably going to give you what you want .

Drills might have the depth of cut you need but as you stated will want to pop into the previously drilled hold. Trying to mill with a drill is also a problem since they are very weak with a side load put on them. Also be aware that a normal style drill is only the spec'ed size at the tip, the rest of the length is slightly smaller.

End-mills will cut the material and irregular shapes fine but you're asking for a tool with a 20 to 1 aspect ratio (20x the diameter of the cut). The highest standard tool we make is 8 to 1. Even if we made a custom tool you would have a very hard time using it. Any runout in your spindle or inconsistency in your material would break the tool.

[Bigbloke]

Just a thought but...

Could you cut several thinner pieces with through holes and then build the part up to get the depth of hole required. use a pair of holes to keep each layer in registration while the glue dries.

That way, you can be left with arbitarily deep irregular shaped holes, no impossible tooling required and could then re-machine the outside shape of the layered piece to get larger scale features as required.

Paul

[jonboycnc]

TDA: about the drill bits slipping into the previous hole. What do reckon the maximum overlap between holes would have to be to prevent this?

Bigbloke: that's a really useful idea - thankyou. I want to let that stew a bit.

[escott76]

Originally Posted by jonboycnc TDA: about the drill bits slipping into the previous hole. What do reckon the maximum overlap between holes would have to be to prevent this? Bigbloke: that's a really useful idea - thankyou. I want to let that stew a bit.

Drill bits follow the point, so they can wander if the cutting edges are not sharpened evenly. Once you start breaking into another hole all bets are off as to what the drill bit is going to do. Especially with the small sizes you are talking about I wouldn't try to overlap at all as they are very flexible.
The features you describe are difficult to make at best. I would even look at getting some of the features laser cut, although that has it's downsides as well, and might not even work well for this.
The other idea I had would be to fabricate a custom "broach" or sawlike tool, but that would only work if you were doing through slots.

[TDA]

Originally Posted by jonboycnc TDA: about the drill bits slipping into the previous hole. What do reckon the maximum overlap between holes would have to be to prevent this?

I have had customers tell me they have cut slots with drills but have never seen it or tried it. I imagine that it would require a very rigid system and more patience than I have. The one way this might work is if you had a drill made with a fishtail tip instead of the "V" style most have. Although this may put more stress on the tool and cause other problems.

Originally Posted by escott76 Drill bits follow the point, so they can wander if the cutting edges are not sharpened evenly.

Even if you have a perfect bit the drill may move back into the previous hole due to runout in the spindle or flex in the machine, table, material, or bit.

The other idea I had would be to fabricate a custom "broach" or sawlike tool, but that would only work if you were doing through slots.

I assume you mean something like a PCB router bit. Where you have many grinding teeth to slowly take chunks out of the material. There are 2 problems with this. First cutting plastics with a grinding tool will almost always melt the material. Second, at those aspect ratios you still have the issue of the tool breaking taking even the smallest bite. Although I may not be grasping what you mean by a broach or sawlike blade.

With the information that we have I think Bigblokes idea has the most potential to get you what you need. Although if you can tell us more about what you're trying to do someone here might have more ideas or another way of doing it.

[escott76]

Originally Posted by TDA I have had customers tell me they have cut slots with drills but have never seen it or tried it. I imagine that it would require a very rigid system and more patience than I have. The one way this might work is if you had a drill made with a fishtail tip instead of the "V" style most have. Although this may put more stress on the tool and cause other problems. Even if you have a perfect bit the drill may move back into the previous hole due to runout in the spindle or flex in the machine, table, material, or bit. I assume you mean something like a PCB router bit. Where you have many grinding teeth to slowly take chunks out of the material. There are 2 problems with this. First cutting plastics with a grinding tool will almost always melt the material. Second, at those aspect ratios you still have the issue of the tool breaking taking even the smallest bite. Although I may not be grasping what you mean by a broach or sawlike blade. With the information that we have I think Bigblokes idea has the most potential to get you what you need. Although if you can tell us more about what you're trying to do someone here might have more ideas or another way of doing it.

I'm not at all an advocate of using drill bits to make a slot. I've gang drilled thick metal before to make cutting easy, but anything that really requires a thin slot is going to be important not to have ridged sides.
I meant a broach held from both ends under tension, like a more precise version of a scroll saw type arrangement. But as I said, that would require a through slot, which may not be what's needed here.
Given somewhat ideal geometry (ie the slots have open pockets on the ends) one could use a jewelers slitting saw but it's only in a very few circumstances.
Another idea might be to overcut the slot wide, planning for a second inserted piece to be fastened in afterwards. Not sure if that makes sense, but say cut the slot .1" + your slot width, then fasten a piece .1" into there, glue etc.

[One of Many]

Here are a few idea for what is meant by the term "broach". There are several different types, but all cut a profile into or through a surface. Sorry I didn't clarify that in my first response.

Broaching tools

Even a fishtail tip micro drill is not going to have the aspect ratio you need to get a flat bottom in the profile. These circuit board bits are also very brittle and do not take to flexing.

DC

[LongRat]

If a through-hole is required, my suggestion would be something like a diamond wire saw. I was under the impression these were blind pockets though. The only way I know of that might work is to use a rapid prototyping technique such as SLS. If other features of the part require a machined surface, the SLS can be post-finished by machining with no problems.