No matter what machining operation I do for making holes in 10mm PVC , i get a tapered hole. The top part of the hole is about 0.15mm larger than the bottom part.
I have used a few different feeds but no change.
Any ideas?
What type of cutter are you using? Some tools are tapered
You could also be experiencing deflection of the tool as it goes deeper into the material… have you tried a “finish” pass that takes a small bit of material off to see if this improves ?
10 mm is pretty thick stuff and the chips may not be clearing out of the pocket as well
Try cutting a pocket with a smaller tool than the diameter of the hole you are cutting. This will give the bit some space to clear chips and will also mean you won’t be heating the pvc all the time where the bit is in contact with the material.
Agreed, I make all holes with a spiral cut using typically a mm smaller diameter end mill then the hole.
@Alex_Krause
I’m using a 2 flute spiral upcut bit designed for cutting plastic. It produced really nice chips.
I have checked the deflection with g-wizard calculator and it is well below the taper i am seeing. I haven’t tried a finish pass but will give it a go. I am using a dust shoe so can’t imagine chip clearance being a problem.
@Brandon_Satterfield @Ben_Delarre I have tried spiral cuts e.g using a 4mm bit to make a 6mm hole. The tapering is less as a percentage of hole diameter than using a 6mm bit so perhaps this is a factor.
@Jeremy_R you don’t mention if the top or bottom of the hole is the right size? Also is it perfectly circular?
@Ben_Delarre The top and bottom of the holes are both undersized, but perfectly circular.
By the way, I have measured backlash to be 0.1mm for x and y axes. The tapering still occurs whether i have backlash compensation turned on or off.
@Brandon_Satterfield So lets say you want to cut a 10mm diameter hole. Do you first spiral cut to 8mm width using a 4mm bit and then plunge cut using a 10mm bit?
oh if they’re both undersized and the top is larger than the bottom then what you have is tool deflection.
Increase spindle rpms and (more likely) decrease feed rate and pass depth. As the bit is moving into the material its flexing, the bottom is flexing more than the top and thus you’re getting a tapered undersized hole.
OK let me give this a try
Check out @Brandon_Satterfield 's great guide for a good read on feeds and speeds, really is an art more than a science on hobbyist machines sadly: http://www.smw3d.com/blog/what-is-the-right-feeds-and-speeds-for-my-cnc-router-kit/
@Ben_Delarre
You were right, it was a deflection issue. I was cutting the PVC with a 1.5mm depth of cut. As a test, I changed the depth of cut to 0.1mm. There was basically no tapering! The hole was still undersized because I previously oversized the tool diameter in CAM. Once I adjust this back down to the right diameter, I should be ok I reckon.
Nice. Out of interest what speed and feed and diameter bit are you using with that 1.5mm cut? I think @Brandon_Satterfield has a spreadsheet floating around somewhere for people to record their settings and results so we can start to build a record and maybe an estimator that works for hobbyists. Might be worth checking out.
I was using a feed of 600-1000mm/min and spindle speed 12000rpm for the 1.5mm depth of cut. Was producing nice chips though.
@Jeremy_R great feedback there chief!
@Ben_Delarre is correct there is simply so much too this. I have found now that making a single part is a very time consuming process. Related, if I were cutting a 10mm depth hole, I would look at my tool selection and see what length cutter I have with a flute length as close to this length as possible. In example if you are using a 17mm flute length with 20mm hanging out tool deflection is going to happen at any aggressive speeds. I would look for a 12mm flute length.
Feeds and speeds calculators. The reason for the article and the spreadsheet, which unfortunately seems to have died now, was to try and gain knowledge for just this instance.
Might suggest, backing off RPM and travel speed. I rarely ever cut on an OX at full spindle speed. Try somewhere around 10k with 400mm/m. Spiral soft at ~3 degrees vs 30. Make your passes light, .4mm or so. Then move up in travel speed and depth of cut till your happy.
Some of this stuff is simply experience drawn from experiments just as you are going through. If we could get enough data feed on the spread sheet a lot of the guess work would be removed.