INACCURACY POCKETING AND PROFILING CYLINDRICAL HOLES (instead of using drill)

[AvB]

When I do the alignment dowel holes around the flanges of the model aircraft moulds, they vary in size depending on what the guy uses for his alignment dowels, e.g. some are for 1/4" tubing, some for 10mm, etc. I don't have drills of the right size for these (or not with enough flute length anyway - the material depth is about 42mm). So I pocket or profile out the hole using an end mill cutter that's smaller diameter than the hole, with flute length greater than the hole depth. For example, today I was doing 10mm holes with a long 8mm 2 flute cutter. I'm always cutting Corian or Freestyle solid surface materials.

The problem is that the holes always end up undersized compared to the hole in the drawing. I have to compensate by drawing holes of slightly larger radius, which often involves a lot of trial and error doing test holes till I get the perfect final hole size. Today I had to use drawn holes of 5.10 radius to get the holes to snugly fit a 10mm rod. I use slower feeds and speeds, and it doesn't help if I turn the Mach3 CV settings right down (eg distance = 2, degrees = 2, almost like G60).

Any ideas?? It's probably some basic thing that I just don't understand that I shouldn't do.

Thanks,
Andrew

Similar Threads:

• Retain defaults in profiling, pocketing etc dialog, being able to enter defaults
• Madcam pocketing and profiling bug in latest update?
• Need Help!- How do I remove unneccesary Z axis retract moves when profiling or pocketing
• Need Help!- Profiling cutting holes.
• Drill holes with end mill or twist drill ?

[Jim Dawson]

Above you describe using an 8mm tool bit........But is is actually 8mm? Maybe it's actually 7.95mm That's what cutter comp is for. Or just tell the CAM program that you have a 7.95mm cutter( or whatever the actual size is). I have seen new bits as much as 0.5 mm undersize.

[GJeff]

Jim is correct. Almost always, when the shaft of the tool is equal in size to the cutting diameter, the cutting diameter will be smaller than what is listed. You can try to measure them by hand to get a rough estimate with calipers, but I'm sure there's a better method.

The other issue is tool deflection. This will make your holes smaller and your profiles larger than they should be. This is not something you typically compensate for - you just make sure your feeds are right to keep it super low. Unlike a cutter being undersized is not a problem for accuracy once you know the size, but even if you know the exact tool deflection, the fact that it happens at all sorts of wonky angles makes it not appropriate for any sort of simple compensation.

Backlash is another possible contributor. So is being out of tram. OI - this machining business is complicated stuff

[AvB]

Thanks gentlemen, I hear what you're saying - good advice and much appreciated. However I feel that something is going on ... the cutters measure up at 8.00 with the Verniers - the one I used yesterday was a good quality Garr. But with a very long fluted section and 2 flutes I guess there's not a lot of material there to provide stiffness. However I've used the same cutter for profiling out inserts and pockets which have turned out really accurate and fitted together perfectly, so I have had no reason to doubt the cutter diameter.

Cutting the holes at only 11,000 rpm, 900mm/min X and 500 Y feedrates and with a stepdown of only 1.5mm in a plastic material really isn't putting enough load on the cutter to deflect it (I think?). And the machine is a very very rigid gantry, with very little deflection. A difference of 0.2mm diameter seems a fair bit to me.

[Jim Dawson]

It's really pretty difficult to interpolate an accurate hole, especially small ones with any CNC machine. There are exceptions to this, but those machines cost north of $1,000,000. I can pretty well count on my milling machine interpolating holes 0.025mm out of round, and I have to make adjustments to the CAM program cutter comp to get it nominally on size, and I have 1um scales on my machine. My router is the same, it requires adjusting the cutter comp in the CAM program to cut holes on size, and it also has 1um scales on it.

If I need an accurate hole I bore or ream to size.

What might help you is to make a couple of spring passes as a finishing operation.

[GJeff]

.2mm off on a 10mm hole is pretty bad. The last time I interpolated a hole that bad it turned out I forgot to tighten the nuts on my vice ><

Something is wrong, I agree. I'd double check your backlash and make sure your gibs are tight.

If a spring pass helps that means its a deflection issue, but you really should never have to spring pass in soft material. I hate the idea of spring passes ever, really. A conservative finishing pass is far better.

Like Jim said, you can't go wrong with boring or reaming when accuracy is needed. But I wouldn't settle for such poor interpolation. You've got some debugging to do.

[Gregore]

I have never had issues with madcam not producing a accurate hole for pins in the 1/8 range using standard slip or press fit numbers .

So I suspect your machine or cutter is off

And yes .2 mm is massively off over 10 mm , if my slides were off .2 over 300mm I would be worried

Not knowing your machine I wonder if something about your settings for acceleration or some other such perameter is off and is effecting small holes more than the rest of your project.

Try running much slower, if the results improve you have your answer

[RCaffin]

Have you thought of buying the right sized drills, getting rid of all the faffing about???
(But not Chinese drills - they can be ... wrong.)

Cheers
Roger

[Dan B]

Think of deflection not from the standpoint of the tool "bending" away from the material like you get cutting steel, but think of it as the soft material pushing away from the cutter then springing back once the cutter passes. We see this happen all the time cuttings soft plastics and nylon, especially if the part is thin.

I think your 900mm/m is too fast, but you said slowing down doesn't help. If your machine supports cutter comp, as Jim suggested above, this would be very beneficial for you in these cases. You could model your holes on size, then make the perfect fit through your controller.

If time is important to you, getting "precision" one-shot drills would make this a breeze. You don't need to spot or ream. Just drill (at crazy fast speeds) and the hole is round and on size. We do this in 4140 steel (a tool steel) all day long. It's a little scary at first because it seems ridiculous to drill that fast, but it works and the drills last a very long time.

Dan

[AvB]

Thanks. Yes, I should buy the drills. However my CNC adventures are infrequent and the holes are just a final step, so although it's mildly annoying it's not a big deal to fiddle around with test holes till I get it right. I'll get some drills next time I make an order. Can you recommend the type of drill and a supplier - assuming I need to drill up to 45mm through Corian?

[Dan B]

I'm not directly involved in tooling purchases but I believe we purchase OSG and Emuge drills.

[williamsmotower]

In Mach I sometimes use the Newfangled widget. Try interpolating a hole that way to check it against Madcam. For some reason my holes turn out much better quality with the widget than they do with Madcam. I don't have size issues, just finishing issues.