Can you do 2- z axis
 

I was worried can you have a machine with 2Z axis One for drilling 5 mm holes and one for cutting. I think about a 5 x 10 cutting area

There is someone here who has, I believe.
Room for dust collection becomes a problem, if I remember correctly.

Yes, yes I have.
Dust collection had to be reduced to a 2-1/2 hose, but in the y-car bay i had:
1) Porter Cable 7518 router on extended z axis
1) Standard z-spider with air drill mounted as far off center line as possible to make room for dust collection.

I don't have pictures, it was a limited specialty use years ago, but the y-car is designed large enough to hold 2 spiders back to back

On this matter Sean, how did you make the software play nicely with two Z-axes? In the CAM program and in Mach3?

dual z axis machine workarounds
 

Alan,
I did a really crude work around in the two different times I did it.

1) I did two individual tool path files and ran the air drill Z axis with that AXIS plugged in to the SINGLE wire feed for that stepper, then just quickly re-patched to the spindle z on the second pass. This is all due to the fact that Mach 3 does not support more than 1 z axis. THIS USES two (1) stepper motor per z axis for a total of two on the machine and using ONE driver in the cabinet.

2) the best solution so far has been on the second z, I just used an air cylinder with hard stops to manually adjust the depth to drill and used the relay out on the PMDX board to "fire and drill" and the appropriate times, which allows for only 1 tool path profile, but a longer set up time for the machine. I my case, I was only using it for 5mm drill and a 7mm depth, so it as an easy accessory. THIS USES two (1) stepper motor per z axis and one AIR Solenoid activated by the PMDX on a fixed stroke and retraction cycle determined by hard stops. (I'm going to find the link and add shortly of the video I used for support)

3) option that I did briefly is the following:

You can set up a macro to swap the axis. Say your drill is the B axis.


In the macro, put

SwapAxis(2,4)

and call it before driling and Z commands will now move the drill.

After drilling, call another macro with

ResetAxisSwap()

I'd recommend using one offset for routing and another for drilling. So if you use G54 when routing, you need to call G55 when you do the SwapAxis. The G55 would contain the offset info from the router to the drill. And when switching back, call G54.

One issue you might have is if you use the Zero axis buttons, you'll be changing the G54 or G55 values, which you don't want to do.

You're going to have to learn to write simple macros to do this.

You can use this script which moves all tool number 2 moves to other axis than Z, just be carefull not to load the modified code twice and parse it. I made two buttons ... simple LOAD and LOAD dual spindle code to the screen

http://www.machsupport.com/forum/ind...html#msg159843

thats how I would do it and did on this machine

http://www.mechmate.com/forums/showt...ghlight=skopje

VIDEO