KX1 CNC Mill Clearance Offer

Andrew,

If I am not mistaken your hobby CNC mill is a big Tormach. I have tried to emulate your impressive feeds and speeds on my much smaller Emco F1, usually with disasterous results. We all get different mileage from our different machines

Slower is always safer and time is not money to the hobbyist..

Mike

I still have X & Y set at 1500mm/min which are the ones that will be doing most of the feeding and the slower Z is hopefully a temporary solution to the stalled motor. need to check the code but think this nameplate was done at 750mm/min feed as its only PVC facia I'm practicing on.

I did say in my previous post that I had a dti on the head and was able to spot when it did not ramp down to the correct position.

Quick update, video to follow later

The settings for the 3mm cutter were left as default in Vectric Cut2D and they were 12000rpm, 30" vertical feed and 100" horizontal. Settings on machine means it actually runs at 5000rpm, 500mm vertical and 1500mm X&Y which seems right as it takes about 4 seconds to feed along 100mm. Should meet Andrews approval

I did find something loose last night and tightened that up and have run the nameplate code 3 times straight off this morning and no errors on height so will run it a few more times later to be sure. Also a lot less backlash when jogging Z.

Here is the video

I was over conservative with the ramping down and could easily have done the full 2mm depth in one pass rather than two 1mm deep cuts but it's early days and lots still to learn but hopefully moving fast enoughto keep me in Andrew's good books.

This is a Vectric thing, one of the reasons why some preferred Dolphin. It adds a few extra seconds/minutes to the process. However, Vectric was found to be easier to learn/deal with and in our opinion - better supported - and it is based in the U.K., even though Vectric's biggest customer base is in the U.S..

Ketan at ARC.

Correct, although I wouldn't call the Tormach big. Although the same nominal horsepower as my Bridgeport I found that the best way to maximise metal removal rates on the Tormach was to use relatively small cutters at high spindle speeds and proportionately high feedrates.

Andrew

Jason, I assume that your 1500 mm/min is the "G00" speed? Though it might work on pvc that would be very fast for metal I think.

So far so good. Although I never expected CNC to see the light of day in your workshop!

Definitely could have done one pass at 2mm. I'd agree that the toolpaths looked a bit odd. It wasn't clear from the video if the initial engagement is just a straight down plunge? I normally ramp, or helix, the cutter down to depth. If you plunge, even with a centre cutting endmill, the centre is still cutting at zero surface speed. I ramp down at about a third to half of the normal cutting speed - for any centre cutting endmill there's only one edge that actually cuts to the centre. Another little oddity in the video is that in clean up the cutter seemed to plunge into the middle of the remaining material and then move outwards, leaving a very thin wall. I'd expect to do the opposite, move to depth in an already cut area and then engage and work inwards. But of course that's purely a function of the CAM program.

While in theory you can run the cutter at very high surface speeds with plastics I've found that in practise you can end up melting the plastic. So I tend to be cautious on spindle speed, but to compensate you can increase depth of cut and chip load to values you'd never consider for metal.

We expect to see the evidence at SCMTEG in a couple of weeks!

Andrew

Dont know the first thing about CNC but watched the video and it impressed me.

Looking at the above picture of the nameplate, the background looks very clean and I cant see any evidence of variation in the depth of cut, I would be well pleased with that.

Ron

Edited By Ron Laden on 28/02/2019 16:25:57

Edited By Ron Laden on 28/02/2019 16:26:45

John Go and G1 are both at max in the code.

Andrew, it did ramp down before I got from mouse to camera, I had it set to ramp down over 25mm which again was too timid but better safe than sorry, it did it in the y axis along the short right hand side then moved off around the rectangle. looks like it ramps in line 220 I'm using a HSS F3 type cutter.

Well as it was free it would have been rude to say no, in my defence it is going to have to sit in the woodworking workshop not the engineering one so not really in the engineering workshop.

I have run the code 10 times now and dti was still spot on zero at the end so fingers crossed

Jason, good news all seems to be OK, like others have said odd coding in the program, could you have used a 4,5 or 6mm cutter to reduce machine time ?

Emgee

Ron, I think you posted while I was typing, yes the bottom looks good with no evidence of cutting at different depths.

Emgee, I don't think anything smaller would have fitted into the "S" If I had set it to ramp down over a shorter distance and set a bigger overlap then that would have speeded things up but at the moment things are moving more than fast enough for me to keep up with.

I don't think it was coding as the error crept in in different places and was not consistant, the ball screw nut was tilting giving a lot of backlash and I think also locking up the screw as it was canted over during high speed movements.

I find it interesting the new software with high speed machining . Even though at times the cutter seems to be cutting too much air, in some cases it actually becomes faster and better for the machine tool life. One example is we had a part and the corners has a 0.5mm radius. The software used to slow down and then speed up trying to get around the small radius. The new software as it came off the end of the part did just over 1/2 of the radius and did a circular path then entering and finishing the other 1/2 of the radius and then goes down the next side. The machine did not bump around as much, the part looked nicer, and the time to make it was actually less. Not what I was expecting at all. Have fun Jason

Neil

Looks like the ramp is line 220 and 230; it goes down by 0.5mm in 25mm and then down another 0.5mm in 25mm in the opposite direction. I normally specify a ramp as depth and angle, arbitrarily 10 degrees. If the CAM program can fit one ramp that's what it does, if space is tight it zig-zags. For pockets like the nameplate I prefer to follow a helical path. Roughly the same; specify the depth, helix angle (10 degrees again) and a radius, just less than the radius of the cutter.

I think high speed tool paths would be better described as constant engagement. The idea is to keep the engagement of the cutter to the work constant, so the cutter is always operating at maximum metal removal rate. The problem (as I've found) with conventional toolpaths is that you set a depth of cut and width of cut. So far so good, but at the end of each straight line the cutter plunges in full width until the width of cut is reached. And if the path narrows the cutter just ploughs through at full width. So you have to back off the parameters so the cutter doesn't break under these conditions. Which then means it's not maximising metal removal the rest of the time.

I looked into updating my CAM program to include high speed paths, but it was more expensive than I wanted to pay. However, I've had some recent enquiries that may lead to a substantial amount of design and CNC machining, in which case I'll go for the upgrade.

Andrew

That's some feed rate. The highest G0 rate on my KX1 is 1000mm/min and my G1 rate rarely gets above the low hundreds. I work mostly with small cutter sizes of 0.5mm to 2mm and with a max spindle speed of 7000, feed rates tend to be in that low region. I'm just trying to visualise my KX1 working at 2500mm.min.

Jim.

Edited By Jim Guthrie on 28/02/2019 22:42:33

Edited By Jim Guthrie on 28/02/2019 22:43:01

Jim, As I said the preset speeds for that cutter in Vectric were 100" or 2540mm/min. with my X&Y set at 1500mm/min that was the max it was able to move at.

Jason,

I used a feed and speed calculator some years ago to get the optimum feed speeds for my small diameter cutters. I can't remember which actual program it was but it certainly cut down my cutter breakage - before that it had been an expensive exercise finding out the hard way. I've just had a look at another feed and speed calculator available online and for a 3mm diameter cutter with a max spindle speed of 5000, which were your settings, the feed rates are well down into the low hundreds. It doesn't cover plastics but I usually double the feed speed for brass or aluminium. The problem with plastics is that a calculated high feed speed is useless since the material will melt, or just distort in front of the cutter. I do a lot of machining of thin styrene sheet and that can happen. The plastic sheet can also lift with the spiral action of the cutter, overcoming your method of holding down.

https://littlemachineshop.com/mobile/speeds_feeds.php

For my small size mills I am way out of the manufacturers' specs since they expect me to have a spindle speed well into five figures.

Jim.

Edited By Jim Guthrie on 01/03/2019 08:33:23

I've played about a bit with some different feed rates today but this stuff seems to prefer it fast as I get a rougher finish and more burrs when feeding slower. by way of comparison if I were profiling this for work I would be using a router at 20,000rpm with a two insert 19mm dia cutter and hand feeding at a fair pace.

A bit more pocketing and profiling to get a feel for the machine and Cut2D

Followed by getting closer to actually making something that could be used. It was not drawn quite symmetrically and I only eyeballed it for the second cut from the other side hence so spokes don't quite line up though that should make for a good representation of some of the castings that are about in the hobby!

Still retained by tabs left around the edge

And popped out of the board

Climb or conventional milling? For some plastics climb milling is worse than conventional.

The plastic may be melting slightly? Looking at an acetal part I've just re-quoted for work I'm running a 4mm cutter at 2800rpm.

Andrew

The CNC is climb milling but conventional hand feed when routing. The facia has a foam type core so that is part of the reason it looks rough, it's not solid UPVC all the way through.

I've had the 3mm 3-flute cutter running at 3000rpm today anf feeds between 600 and 1000mm/min