[drakesis]

Why is my machine skipping the corner of a square?

[alan_3301]

looks like a combination of acceleration too low, and long bit deflecting?

It look like some results I was getting when I used a harbor freight 1/4 HSS bit that was like 4 inches long

It would also be good to make sure there isn't excessive backlash on any axis, and that you don't miss any steps while cutting.

[drakesis]

It is with a 1/4" double flute upcut end mill. Calculating the chip load it should be running at 112ipm, but it's even more awful at that feed rate.

It's probably 2-3 inches long, didn't think about deflection. Wouldn't have thought cutting 1/8" in wood would cause it to deflect?

Backlash seems fine.

[ger21]

What are your acceleration settings in Motor tuning?

[alan_3301]

I'm not familiar with the mach settings, but set your accel to 20 or higher if your machine is up to it. Otherwise research mach3 options for path tolerance, so it will slow down in corners to not deviate from the path.

With your dial indicator, check the runout of the bit, to see how much it wobbles.

[ger21]

I assumed you were using mach3, but apparently you're not?? What's a TM machine, and what control is it?

[drakesis]

I assumed you were using mach3, but apparently you're not?? What's a TM machine, and what control is it?

Sorry, I guess I didn't say in my first post. TM is a Torchmate. I believe the control is a relabeled Flashcut controller.

[HungryArie]

Take a look at this site: https://www.cncci.com/resources/tips/g61.htm
I think your cnc skippes corners because your controller has a lookahead feature. It shortens the corners to keep on speed.

[jch13]

I have a dial indicator for checking runout, not sure how it will help me in this situation?

This should be outlined in your controller manual go there for a detailed write-up. But a REALLY quick and dirty is:

1. Setup and zero the dial indicator on an axis. I start with the heaviest axis.
2. Create a program to jog 2-12 inches and return to zero.
3. Run said program to adjust (in this order) Start/Stop Feedrate, Maximum Feedrate, Ramping Rate
4. Find where each of these settings start to miss steps (should be very obvious on dial indicator) and then set to final value to half of the value just before skipping occurs. i.e. set maximum feedrate to 499, ramping rate to 499, and then adjust start/stop feedrate until you see skips. Try 150ipm (that will likely skip) then halve it to 75ipm, if this sips halve again, if it doesn't skip split the difference and try 113ipm, etc. Repeat until you're making small changes. I decided to not adjust finer than 5ipm increments. Lets say you find that 100ipm start/stop rate doesn't skip, set your final value to 50ipm to be conservative.
5. Run a rapid program through the entire range of the axis. This will help ensure that nothing is binding or skipping through the whole range of motion. My machine was easily repeatable to 0.001-0.002in without any special effort.
6. Repeat this process for all axes.

The purpose of this is to make sure that none of your settings will cause an axis to skip steps or slip during normal operation. It might not be the cause of this issue, but it's a most-do to properly setup a machine.

Don't remember, I was doing alot of tests. Probably between 8K to 10K, trying to get a good chipload set. But it's difficult to do as the TM machine maxs out at 150ipm.

That is just too slow IMO. Remember - a CNC router is a very flexible machine. Thus to must de-rate your cutting power substantially. G-Wizard's calculations de-rate mine to around 0.1-0.2HP vs the 2.25hp router mounted on it. I also aim to keep tool deflection around 0.0005in, which usually entails cranking up the cutting RPM to reduce chip load. A carbide cutter can take the heat, just make sure you're not smoking the wood!

The last time I did a large piece of plywood I did the following:

Ultra-conservative
http://i.imgur.com/L0DVbcB.jpg
100ipm feedrate, 10ipm plunge, .063in DOC, 24krpm, 1/8in 2-flute carbide downcutbit, ~60min cut time with super-inefficient rapids, was able to halve this by using settings similar to those below. Again, inefficient rapids were the biggest time-suck, my CAM software is awful at that.

Considerably more aggressive
http://i.imgur.com/FgtZxiL.jpg
180ipm feedrate, ~20ipm plunge, 0.190in DOC 24krpm, 1/4in 2-flute carbide upcut bit, ~20min total cut time

The thing that REALLY sticks out between these and yours is how clean the edges look. I think this has a lot to do with your feeds/speeds setup being totally out of whack. My as-cut edges are nearly perfect, they only needed the lightest of sanding (or even just a finger nail) to clean off.

I think you should try settings similar to these and then get back to us. If anything it will eliminate feeds/speeds as a culprit.

The machine is square, Haven't thought of doing a rectangle..... I show run a test with one going in X and another going up on Y....

My idea behind checking every area of travel will help determine if the error is programmatic or mechanical. You could rapid through every section of every axis to check. Or cut out a large piece. Perhaps even try cutting out a large circle. Each of these test will tell us something.

Yes, HSS Endmill, 2in is correct. Holy crummers! That would mean 40 minutes or more to cut a 2'x4' sheet of 1/2" plywood.

Should I be using a different cutter(s)? (Maybe that's another post......)

Yes. Carbide or go home IMO (for a router). It's the only real way to paly to a CNC Router's characteristics - high RPM cutting and stiff tooling to help make up for an un-stiff machine.

[drakesis]

I hope to have some time later this afternoon to do more tests... I will definitely try out a large circle, etc... see what it tells me!