Home lost during 3D cut

[Coogara]

I'd appreciate poiinters on what to consider concerning losing home position during a 3D cut. I've cut a number of 3D models successfully, but at 10"x10" this is the largest and longest running cut so far.

The roughing and finishing instructions were combined in a single file using the 1/8" ballnose that comes with the Desktop model. The roughing pass dug out a maxiumum 1/4" depth and the finishing pass was digging out a further maximum 1/4". So the deepest parts are around 1/2". The machine comes nowhere near obstructions or the physical limits of the machine.

The roughing pass was well over and completed successfully. The finishing pass was underway. About 25% of the way through the finishing pass the machine abruptly lost home position. Suddenly it was cutting with an offset of about -1.25" in X and maybe an 1/8" in the Y.

As I was monitoring the cutting via web cam, I cannot say whether there was noticable shuddering at any point that may have indicated a sudden loss of position. The machine continued cutting for some time after loss of position with no further indication of loss of position.

What do you think, guys and gals?

Thanks

Graeme

[Brady Watson]

What was your X,Y move & jog speeds, and what RPM were you cutting?

-B

[Coogara]

Hi Brady,

I'm still a wee babe when it comes to things in the CNC world. Lots to learn despite some early successes. I'll chalk this one up to a good learning exercise. What I'm hoping and expecting is that the issues lie with my settings and not a fault in the machine!

I had not changed these from the installed defaults:

Move X/Y: 4
Jog X/Y: 4

I also noticed, somewhat belatedly, that the pass depth for the 1/8" ballnose was set to 0.3". I usually try to take some notice of the settings for the bits but overlooked this one. Is 0.3" too aggressive?

Thanks

Graeme

[Brady Watson]

Graeme,
It could be that your 3D roughing pass did not clear out enough material for that 1/8" ball finishing pass. The idea is to clear away as much as you can with a square end tool & a 3D roughing strategy, usually leaving .02-.04" of 'meat' for the finishing pass to leisurely shave off. I prefer to do a roughing pass as well as a profile pass around the part in order to get rid of any potential for there to be shock loads on the bit as it gets jammed into surrounding material (not good!).

So...rough out with a square end mill and clear away the bulk of the material. Switch your tool to the ball and do the finishing. There is nothing wrong with setting the stepdown on a tool that will ONLY be used on a 3D toolpath, because stepdown is completely ignored. You could have stepdown set to 3", and it will only go as deep as the relief is high. However, if you use that 1/8" ball to do a profile cut, it will go that full 3" deep PER PASS(!) which I can assure you would be fatal to the bit and your collet nut!

In terms of cutting speed, the jog speeds are fine, although I would pull the Z speed back to 2. The MS will be changed in your PartWorks file. The speeds are set in the tool database. Feel free to change them - and please get this - The speeds listed in the tool database are absolutely 100% NOT suggested, recommended or correct speeds! I have been on them to change this for months. There is NO practical reason why an 1/8" ball should be run on a Desktop @ 7,7 inches per second. A more appropriate speed setting for that bit would be 2,1 (XY, Z speeds respectively) or even 3,2. Faster than this and deeper than is reasonable for this type of tool WILL overload the motors and cause them to stall. You cannot apply a 2hp load to a 1hp motor and expect it to work. Same idea here.

Try fooling with the speeds and slow things down a bit. I'm all about quality, and until you get that 3D 'takes as long as it takes', you won't full realize that operating faster than the tool really wants to go just makes for poor quality parts. The faster you go, the less power you have...and the opposite is true with stepper motors. Learn to listen to what the tool is telling you...you will learn volumes that cannot be taught any other way.

Does that help at all?

-B

[myxpykalix]

Graeme,
Here is a practice that i started doing and it has gotten me out of hot water on more then one occassion.

I always use the center of my material for my X,Y Zero position.

So in case i lose communication or whatever i can always find X,Y Zero even if it has been cut away.
I do a C3 and find 0,0 on my table
I then load my part where i have made a X on it to locate the center of the part.
I then manually move my carriage and find the center of the X on my material with the bit.

I go to the computer screen and write down my X and Y position on the readout

I then Zero X,Y

Then I do a C2 to my material surface. I make sure to have extra material outside the boundries of my cut to Re C2 if needed.

Now if you have any issues or lose position all you have to do is to go back and do a C3
then do a MX (your written down coordinate)
then do a MY (your written down coordinate)
and you are now back to center

[Coogara]

Brady, after this issue I started playing with my design to use an end mill in the roughing pass. I totally concur. Not only will they pull out more material but the roughing will be faster. I will change the Z speed to 2 and, as you and other have suggested, substantially ignore the tool database values. All good advice and much appreciated.

Jack, I like your suggestion about obtaining the relative position of the spindle and recording it prior to zeroing X/Y. Although power is more reliable in my area than it once was, we have a history of losing it in the middle of things. This would get me out of a lot of trouble.

Thank you both for some sound suggestions.

Cheers

Graeme