Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: TonyP on November 01, 2007, 04:07:47 PM
-
I've been trying to set up a simple gang tooling plate on my Boxford TCL125. This requires the use of tools from both sides of the work. I assumed that this would mean setting Rear or Front in the tool table, and setting up the offsets in a similar way to single-sided cutting. I get very strange results when I try this. The manual does suggest that switching toolposts is not a good idea but I can't see any other way to set things up.
Has anybody done anything similar ? I'm only doing this to give me something to play with while I think about a tool changer. To my great regret I passed up the chance to buy one for £90 a year ago!
Tony
-
Tony,
Have you seen my little video on the Mach Youtube site?
http://www.youtube.com/watch?v=Ehit1ip1LfM
I don't set set it up as front and rear toolpost, just use X and Z offsets. On the toolplate the "front tool" is cutting upside down - easy!
In comparison the turret is slow because of the G00 moves to change from turning to drilling and time out to move to a safe position to index.
Regards,
Ian
-
Ian,
thanks for that. I still don't really understand how you're managing it. Which is your Master tool? I've been using the uppermost as master but when I come to the lower tool the offsets don't seem to work out.
The way I envisage toolplate operation is that, when a tool is called, Mach knows where to put the tip (because of the offset) and(because of the front, rear info) which way the in-feed should go. Z of course works OK as there is no difference.
This is all new to me. The good thing about the TCL is that it's small enough to live on a trolley in my nice warm office while I learn, instead of out in the cold main workshop.
Tony
-
Tony,
The way I set it up is to use, say, the turning tool and jog it to touch the end of the bar and set the Z on the Mach display to zero. Touch the tool on the OD and set the X display to zero. This gives me the 0,0 from which all other tools are displaced like the origin on graph paper. For example, I would then jog the drill to the centre of the bar end and read off the X and Z values.
These are then used in a G00 move in the G code. Repeat this jogging to get values for all the tools and write all the G code setting depth of cuts and feed rates and making sure there are no collisions.
Cycle the G code cutting air, make any corrections, then cut metal. All that remains is to tweak the code to get exact sizes and the job is done!
Hope this helps.
Regards,
Ian
-
Ian.
I think I've got it. I wasn't changing the sign of the part size when touching the bottom tool.
Also I need to do the same for the 'x' co-ordinates in code generated by the wizards when using tools below the centre line.
Would it be possible to see your code for that part (or something similar) to see if I've got the right idea?
Tony
-
Tony,
At the risk of boring people and showing my scruffy G code in public, this is the text for the collet blank in the toolplate video :-
(Collet2)
(22mm Stickout)
(Touch OD X 00 Touch end Z 00)
n10 g90 g21 g95
n20 S2000 (Manually set at the moment)
n30 g00 z 00 x1.00
n40 g01 x-6.75 f0.05 (Face)
n50 g00 x-1.50
n60 g01 x-0.85 z-0.50 f0.025(Chamfer)
n70 g01 z-10.00 f0.05 (Turn)
n80 g00 x-0.25
n90 g01 x0.50 z -10.75 f0.025(Chamfer)
n100 g00 z-16.5
n110 g01 x-1.00 f0.025(Form chamfer)
n120 g00 x1.00
n130 g00 z-1.00
n140 g00 x35.41
n150 g01 z-19.00 f0.10 (Drill, note that it is a left hand drill with rake modified for brass)
n160 g00 z-1.84 (Extract drill)
n170 g00 x44
n180 g00 z-15.00
n190 g01 x50.41 f0.05(Part)
n200 g00 z-7.50
n210 g00 x15.37(End Stop)
n300 M30
This should all make some sense to you now you've got the idea. For simple jobs on the lathe, I don't use wizards or Lazycam but the little mill is a different ball game.
Regards,
Ian
-
Interesting code, very compact,
Graham.
-
I used fixture offsets before i completed my turret worked - well G54 - G59
-
Ian,
thanks for that. It does make sense. It's a more direct approach than I was trying, and independent of anything but the basic Mach functions. I suppose the virtue of using tool offsets is that re-setting a tool would be easier.
What state is your TCL in? How much rebuilding did you do? I've now replaced all the electronics except the Spindle motor & drive, the axis steppers & the PSU. Having just replaced the axis drivers with some from ARC-EURO, I'm having some fun trying to decide what current to set on the drives. The motors are the originals, one larger than the other, with no sensible ID. I've got them set to x 1.8A, z 2.1A at the moment, but I suspect they should be higher.
Spindle motor control with the Gemini Drive & solid state relays works fine.
Tony
Tony
-
Hi Tony,
what are you using to control the spindle speed?
The large motor is 2.5A and the small one is 2A
Graham.
-
Graham,
the motor controller is the original Gemini. I'm controlling the speed with dc derived from a V to F convertor chip (LM2197). The direction uses the original reversing contactor driven from 2 D2W202F solid-state relays.
I designed my own breakout board, which works fine, but I have found that some printer ports won't drive all the optos. I'm going to add some extra drivers to make it a bit more universal.
Thanks for the motor info. I thought it might be something like that from my measurements on the old unipolar drive. They don't even get warm at the moment, so I'll move it all up a notch.
Tony
-
LM2197? I cant find any reference to that on the web. Is that a valid number?
Graham.
-
LM2917N-8
A national device - got one in my hand.
Tony
-
thanks Tony,
Graham.
-
Tony,
You asked:-
"What state is your TCL in? How much rebuilding did you do? I've now replaced all the electronics except the Spindle motor & drive, the axis steppers & the PSU. Having just replaced the axis drivers with some from ARC-EURO, I'm having some fun trying to decide what current to set on the drives. The motors are the originals, one larger than the other, with no sensible ID. I've got them set to x 1.8A, z 2.1A at the moment, but I suspect they should be higher.
Spindle motor control with the Gemini Drive & solid state relays works fine."
I replaced the round steppers with square NEMA 23 2.5 Amp ones which are MotionKing 1.1 Nm. The drivers I used were 3 Amp 30 Volt £30.00. The BOB was CNC4PC C10.
This setup would run at 1.8 m/min for a G00 move but would stall if pushed any higher. In order to have some reserve power, I am now fitting 2 of Gecko's 203V's and a CNC4PC C11G and the first impressions are realy good. I was able to push Mach3 up to 45KHz and have a surplus of torque, up from 0.3 Nm to 0.8 Nm at cutting feed rates, measured on the end of the ballscrew. The stepper is now running at 1350 rpm max, about 2.5m/min on a G00 move. I am still playing with this setup, so no final figures yet.
The original interlocked fwd/rev contactors are still fitted but I have not needed reverse yet, though I do have a small tapping head to try. My Gemini failed, so I replaced it with a SMC-00 from www.beel.ca. This drives the Lenze DC motor and provides plenty of cutting torque. The C11G will enable Mach to control the spindle speed and fwd/rev eventually.
Like Graham said, just push the amps up until the steppers run hot, then back off a bit.
Hope this helps,
Ian
-
Graham,
My "interesting" code would probably make Art cringe. He has provided all sorts of toys in Mach3 and I didn't use any! Not really worth it for simple, short runs.
Regards,
Ian
-
Ian,
thanks for the code - it all makes sense now. I've even run it and cut a part in PVC. I did have to alter it to suit my axes, however. My x gets more positive as the cross slide moves up - I think yours must be the other way round. I also altered line 100 to a G01 move. With my current motor setup the code takes 35 secs to run, which is not too bad I think.
Tony
-
Tony,
Well done! Have fun and keep us informed. Gecko's on the TCL in another thread.
Ian