Z question

[Island Glass]

I'm wondering how to get my finish tool path to go a little deeper. Occasionally there is still roughing tool marks showing . My solution so far is to loosen the bit and pull it out just a tiny little bit then re tighten but there must be a better way. When I do the touch top I get a number instead of "0" In wincnc if I move the z height a little higher say it's at 6.0 and I move it to 6.1 and zero it goes to 0 instead of 6.1 Seems a little confusing. The shopbot I had to start with would go to Y 0 x 0 and z 0
Also I frequently come back to the CNC and the spindle has fallen down to the stops I.ve started always putting it in park so it doesn't jab the bit into the table or break a 1/16 ball nose Is there a solution to this problem? I assume it doesn't hurt anything if it slides down. I've got leaks in my air system so I can't leave it on all the time. Any help would be appreciated Bill W. Melrose Florida

[Robert Alexander]

I'm wondering how to get my finish tool path to go a little deeper. Occasionally there is still roughing tool marks showing . My solution so far is to loosen the bit and pull it out just a tiny little bit then re tighten but there must be a better way. When I do the touch top I get a number instead of "0" In wincnc if I move the z height a little higher say it's at 6.0 and I move it to 6.1 and zero it goes to 0 instead of 6.1 Seems a little confusing. The shopbot I had to start with would go to Y 0 x 0 and z 0
Also I frequently come back to the CNC and the spindle has fallen down to the stops I.ve started always putting it in park so it doesn't jab the bit into the table or break a 1/16 ball nose Is there a solution to this problem? I assume it doesn't hurt anything if it slides down. I've got leaks in my air system so I can't leave it on all the time. Any help would be appreciated Bill W. Melrose Florida

For a possible solution for your roughing marks, can you do a re-cut with a slower speed and increase your rpm's a little. If not just set your bit on the top of your material and hit the Z, then lower your Z down .02 and hit the Z reset again(this will work if you have set your material height for the top of the material, and not the spoilboard surface) . As for your spindle falling down, cut a block of wood just smaller than the full height of the spindle and lower the spindle down to the wood block, then turn off your machine. For your air leak problem with the air line pressurized you can get some drops of liquid dish soap mixed a cup of water and take a brush and brush it on your fittings to find your air leak. You should then look for a bunch of small bubbles forming where the leak is.

[Gripus]

My first question is...are you using Aspire? When you create your roughing toolpath there is a box in which you enter an allowance or how much you want to leave for the finish cut. I believe it defaults to .020". I would think if you had a very small, or no, allowance there might not be enough material left for your finish bit to cut.

Another question is do you have the Z zero pad? If you don't get your finish Z set exactly as you have your roughing Z there could be too shallow of a cut and tool marks.

If your Z is 6.0 and you move it to 6.1 and hit "zero Z" the display will be 0.00 because you just told your machine its current location was your Z zero (0.00).

For a solution to your drop problem look here (http://www.camheads.org/showthread.php?t=913&highlight=sabine).

Joe

[kenrbass]

I have wincnc on a (Machine) and I'm sure it works the same. If yours is running Mach 3 someone else will have to chime in.

L28z This command will zero the z in the current location.

You may have to do a G49 to get out of the relative z mode.

You can also give the z a number after the command.

If you use L28 z -.1 it will work just like the VA command did in the (Machine).

You can also use L28 x y type of commands if you want to zero x and y

Ken

this post edited by moderator

Moderators note : we provide this forum as a support tool to those who purchase or own the camaster machines, on another note we invite all who are interested in the cnc and uses of to participate in active dicussions of software and operations, we work to keep the issue of machines on the camaster for the sole benefit of the ownwers

[JohnnyCNC]

L28 sets Absolute Zero. It's just like homing the machine. If you have homed it and do a L28 X0 Y0, you've just lost your real position. There's probably a zero button on the WinCNC screen. If so, use that. It will set a Local Zero (a green box appears beside the axis letters). You can turn these zeros off by typing G92 and hitting Enter and you're back to your absolute position.

If you don't have the button, you can do the same thing by typing G92 X0 Y0. You can do the same thing with Z... G92 Z 0. You can also do G92 Z -.1 . That will make the controller think you are sitting 0.1 inches below zero. If you did G92 Z1, the controller will think you are 1 inch above zero.

JohnnyCNC

[kenrbass]

Good info. The absolute, relative, temporary stuff gets a little confusing. lol

I agree doing an absolute on a xy position could land you in trouble with soft limits.

Assume he had a z that went to 2 inches to park after the file was ran.

So if he finished his file and want to take another .020 off of the top, he could safely run a G92 z 2.02 and that would allow him to cut another .020 off of his part right?

Ken

[Mick Martin]

I think Bill is using Aspire, Am I correct?

As Joe stated when you create your roughing toolpath there is a box in which you enter an allowance or how much you want to leave for the finish cut. I believe it defaults to .020

What is the condition of your router bit and collet, could the bit be slipping?

What happens if you create a toolpath to pocket a 4" x 4" 1/4" deep, then remove and reinstall the same bit and run the toolpath again, are you cutting air?

Are you measuring T1 (spoilerboard) and touch top (material) with every bit change?

Mick

[Island Glass]

I'm using Aspire and almost always Z to the top of material with touch pad. I think part of the problem is I'm almost never in exactly the same spot with the touch pad and since I'm using mostly thick rough cut wood then there will always be a little difference in z height. How would I know if the collet is bad and the bit is slipping ? If I change the z height say G92 Z -.01 will I need to undo anything on the next toolpath? I really appreciate the help
Thanks Bill W.

[Mick Martin]

I'm using Aspire and almost always Z to the top of material with touch pad. I think part of the problem is I'm almost never in exactly the same spot with the touch pad and since I'm using mostly thick rough cut wood then there will always be a little difference in z height. How would I know if the collet is bad and the bit is slipping ? If I change the z height say G92 Z -.01 will I need to undo anything on the next toolpath? I really appreciate the help
Thanks Bill W.

Secure a piece plywood or MDF on the spoilerboard then create a toolpath to pocket a 4" x 4" 1/4" deep, then remove and reinstall the same bit and run the toolpath again...... any smooth wood will do.

Examine your router bit shank for marks, grooves or discoloring then check your collet for the same condition. Is your collet clean (no dust) or have any cracks.

Mick

[Brad Knight]

How would I know if the collet is bad and the bit is slipping ? If I change the z height say G92 Z -.01 will I need to undo anything on the next toolpath?

Umm forgive me if I'm wrong... but you have to zero your z on every toolpath. Or should I say, you're measuring your tool on every tool path, but using your zpad to zero your z has the same net effect.

And you should do it at the same spot every time. The idea is that you pick a point in space and when the tip of the bit gets to that point, call it zero - call the same point zero for each bit in the project and you should get much better and repeatable toolpaths.

[JohnnyCNC]

I guess I'm a little wierd here. I zero at the table. That way my zero is always the same. I just plug my material thickness in and let my CAD/CAM software do its job.

This also gives me an extra bonus that you can't get when you zero at the top of your material. I can pull my GCode up in a text editor (like notepad) and do a find in files for "z-" (z minus). If I find it, I know I'm going to cut into my spoilboard. If I zero at the top of my material, I have to re-zero every time I change material thickness. Seems like a lot of unnecessary work to me.

Oh yeah, I use a form of the FTC, so my tool measure is done after each tool change, but it's always done at the same fixed place by the computer and as many times as my multi-tool files call for. I just wait for it to stop, take out the last tool, stick the next tool in, tighten it up and hit enter. The tool is measured, the spindle comes on and it's back digging. All I have to do is make sure I get the right tool in at the right time. Why does it work? WinCNC knows where my table surface is in relation to my switch. It automatically subtracts/adds the distance from the switch surface to the table surface from/to my measured tool length. The only time I have to manually re-zero my tool is if I mill my spoilboard.

Do I sound like I like the FTC system? I don't know how you get that idea!!!

If you have a non-tool changing system, talk to Joey. Have him fix you up. I don't figure you'll regret it. But that's just my opinion.

JohnnyCNC

[Mick Martin]

I guess I'm a little wierd here. I zero at the table. That way my zero is always the same.
JohnnyCNC

Good point ...

[kenrbass]

Johnny,

I made a file to surface my table. At the end of that file, after turning the spindle off and pausing for it to stop, it moves the z to the spoil board (-.020 in my case) and then runs the g37cal file.

This way everytime the spoilboard is cut, it just takes care of itself.

I also put a shortcut key on the screen pulling up a macro that has the flycut.mac file in it.

I work real hard so I can be lazy[embar]

Ken

[JohnnyCNC]

That's a cool mill table file Ken. I like it. You know how far to lower it below zero because that's how much you milled off.

Is your machine a tool changer? If so, you might use the M37.3 to adjust your tools after milling the table. That way you wouldn't have to pick each of them up and measure them again. Say you had taken that .02" you mentioned off. Depending on whether you are using the new tool library or the old style it looks something like this:

Old:
M37.3 S-.02 H0

New:
M37.3 S-.02 T0

Of course I could have this wrong. I suggest you look it up in the WinCNC manual.

JohnnyCNC