X2 cnc finished for now maybe

[Deviant]

I was curious how the surface grinder works.

In regards,
How do you account for wheel being out of square and eventual wear? I've always wondered about that.

Hope you don't mine the slightly off topic question.

Lots of nice add ons, keep up the good work. = )

[hoss2006]

Digits, I did cut the lathe head on another lathe.
you can get the original cast iron version at LMS.

Deviant, I've only used the surface grinder once so far. i just wanted a way to resharpen my planer knives accurately. I square the wheel with a diamond dresser mounted in a small block of steel pointing up ( like a candle in a cupcake). I use the mag table to hold it and run the grinder back and forth (Y Axis) a little at a time (feed down on Z)to true it up.

you can buy relays that will turn the motor on or off through mach. you just have to get one that ir rated at the amp &volts you need or higher &wire it to one of the out put pins that will put out 5 volts when activated. i have bought them on ebay for as low as $11.50 for 4. just type in solid state relays. i have one on my taig now. works great! greg

If only it were that easy.
The X2 electronics that control the motor have safeguards built in that won't
allow the motor to be turned on at higher speeds.
Just like the treadmill controller I replaced my bad board with, "A motor controlled by this board must start at or near zero speed and then the potentiometer can be turned up for higher motor speed, the board will not allow the motor to be switched on at high speed."
If power is cut, i.e. with a relay, the pot has to be turned off then back on to
get the motor back up and running.

Hoss

Greg you should have hit me with a hammer.
It finally dawned on me how that would work.

if I hook the relay up to the wires coming from the circuit board to the motor
and interrupt the power there instead of interrupting power to the circuit board it WILL work by gosh.
I still have to turn the motor on with the pot and set the RPM initially, but after that the relay (controlled by Mach 3) can turn the motor on and off the rest of the day. A lot cheaper than buying a breakout board for $100 or so.
I was gonna have to come up with something for the Automatic Tool Changer I'm starting on. It HAS to turn the motor on/off to change tools. I'll have to do a little checking to see if/how mach 3 can control the speed but that isn't as necessary ( but would be nice) for running the ATC.
I did a little experiment with a wall switch just to see if the relay idea would work
and it did. The motor came on at the speed I left the pot set at each time.
that's another hurdle taken care of.

P.S. got my 4th Axis finished for the lathe attachment.
Now I just have to figure out how to program the freakin thing.

[skmetal7]

that's flipping sweet! have fun trying to program it! i would think oneCNC with the 4th axis option for programming tool paths would work but i'm sure that's wayyyyyyyyyy out of your budget! lol.

i would be concerned with the current draw from the motor when u have the pot set at a certain speed and u turn it on, it could overload the speed control. have u seen http://www.cnc4pc.com/Store/osc/prod...products_id=58
its a controller that u connect to the existing speed controller in your mill, just connect it to where the pot would go and u have a spindle thats controllable by MACH. although i think it takes up an axis.

[hoss2006]

skmetal7, well thats the ticket.
That board should kill 2 birds.
vary the rpm and take the rpm to zero for the tool change, awesome.
And it's in my cheap a*s price range.
I hate to ask what the oneCNC goes for. Didn't see a price on their site.
i guess if you have to ask you cant afford it.
Thanks

[skmetal7]

i think i heard it was $3k, lol! and BobCAD-CAM is a little cheaper, they have an upgrade version for $495 (a hobby version) but i dont know if u can install that without the complete package($1000). http://www.bobcad.com/index.php?sele...e=pricingfull4

[digits]

Hi hoss - I actually have both a lathe and X-2 mill head from LMS - I really like the look of your solid aluminium one though - perhaps I'll build the lathe and have it make parts for its own upgrade!

I like the look of your lathe/4-th axis setup hoss - I'm trying to work out a way to do it with one motor, but I might just try your elegantly simple solution first! After all, I reckon it's being able to switch from milling to turning without touching the work piece that's the useful/clever bit!

Do you get enough torque on the stepper setup to hold the work still against the mill cutting force? If so, what's your belt reduction factor, and how beefy is that huge stepper? I currently have my 4-th axis on a rotary table, but a lathe head would be more flexible as it could do high speed.

As for 4th axis CAM, I'm currently using MeshCAM - not done any 4-axis stuff yet, but I am planning to make a spindle gear with it, so I'll let you know well it works.

Cheers.

[hoss2006]

digits,
I used 2 separate motors for one reason, they were free!
Well I paid for them a while back but they were just sitting around.
I have to try some software to get it going to see how well it holds.
I want to make some wrench flats and see if it wiggles any. It's a 495 oz/in motor so it's as good as a nema 23's gonna get.
I have a 15 tooth on the motor and 27 on the spindle.
Wanted 1 step of the 200 steps/rev motor to equal 1 degree rotation of the spindle. thought it might make programming easier, who knows.

[digits]

digits,
I used 2 separate motors for one reason, they were free!
Well I paid for them a while back but they were just sitting around.
I have to try some software to get it going to see how well it holds.
I want to make some wrench flats and see if it wiggles any. It's a 495 oz/in motor so it's as good as a nema 23's gonna get.
I have a 15 tooth on the motor and 27 on the spindle.
Wanted 1 step of the 200 steps/rev motor to equal 1 degree rotation of the spindle. thought it might make programming easier, who knows.

If you have Mach 3, you could just add it as a rotary axis A, and then just send it to an arbitay angle with a G0 Axxx where xxx is the desired position - but I assume you already know that? If you know the steps per rev of the motor and the gear-ratio of your pulley, you can just add it in Mach 3 as a steps per rev, much like the steps per inch you have for your linear axes - it really is that simple!

If you want to check it it will hold, you could just try mounting some stock, milling some of it off, roating it 90 degrees with a G0 A90 and then milling some more off - if the two sides are perpendicular then the 4-th axis is working - I'd imagine if it's out by a constant factor, the steps per rev are wrong, and if it's out by varying amounts along the cut, it's not holding - but I could be wrong. Have fun!

[hoss2006]

Digits,
I tried using the G0 A90 in Mach 3 to rotate the 4th axis but I must be missing something somewhere,
it rotated and rotated like it was moving 90 inches.
I made sure the 'A-Axis is angular box was checked under Angular Properties but still nogo.
I got it working though.
I set the motor tuning up so the motor spun 1 rev per inch.
the stepper is a 1.8 deg/rev, 200 steps/rev at 1/8 microstepping.
set the A Axis motor to 2880 'steps per' at velocity of 40.
200 steps x 8 = 1600 x 1.8 = 2880 steps/rev.
Now when I program it, .25 in = 90 degrees, .5 = 180, .75 = 270 etc.
I made a little program to mill some wrench flats and the stepper held it great.
cut aluminum .050 deep at 25ipm and it didn't wiggle at all.
made a couple more programs to cut 6 and 8 flats.
wrote a program to mill a 16 tooth timing pulley. just took .015 at 10ipm per pass with .078 endmill.
Looked pretty good. no more buying them for me. used a 90 degree csink to break the edges.
I'll have videos up at Youtube here shortly.
http://www.youtube.com/hossmachine
I can program this way but would like to hear what I missed to use the G0 A90 etc. in Mach 3.
Hoss

[digits]

Digits,
I tried using the G0 A90 in Mach 3 to rotate the 4th axis but I must be missing something somewhere,
it rotated and rotated like it was moving 90 inches.
I made sure the 'A-Axis is angular box was checked under Angular Properties but still nogo.
I got it working though.
I set the motor tuning up so the motor spun 1 rev per inch.
the stepper is a 1.8 deg/rev, 200 steps/rev at 1/8 microstepping.
set the A Axis motor to 2880 'steps per' at velocity of 40.
200 steps x 8 = 1600 x 1.8 = 2880 steps/rev.
Now when I program it, .25 in = 90 degrees, .5 = 180, .75 = 270 etc.
I made a little program to mill some wrench flats and the stepper held it great.
cut aluminum .050 deep at 25ipm and it didn't wiggle at all.
made a couple more programs to cut 6 and 8 flats.
wrote a program to mill a 16 tooth timing pulley. just took .015 at 10ipm per pass with .078 endmill.
Looked pretty good. no more buying them for me. used a 90 degree csink to break the edges.
I'll have videos up at Youtube here shortly.
http://www.youtube.com/hossmachine
I can program this way but would like to hear what I missed to use the G0 A90 etc. in Mach 3.
Hoss

Wow - love the pulleys hoss - I spent ages today indicating my 3-jaw chuck on my rotary table so that I can cut some timing pulleys tomorrow

As for your A-axis setup in Mach 3 -

Your stepper is 1.8 degrees per step - therefore it is 360/1.8 = 200 steps per revolution on a 1:1 geared rotary axis. You have 1/8th micro stepping, so you actually have 200/(1/8) = 1600 steps per revolution assuming 1:1 gearing. Factor in whatever your pulley sizes are, and that should give you the steps per revolution for your setup.

My rotary table has a 90:1 worm ratio - and my steppers are 1600 steps per revolution, so I get 90 x 1600 = 144,000 steps per revolution of the rotary table. Mach 3 seems to take steps per degree so I have 144,000/360 = 400 entered in the steps per box - seems to work fine

[project5k]

somebody get me a napkin.. i'm drooling all over my keyboard...

i cant wait till i can do that kinda stuff...

hey Hoss.... i gotta ask, when you say you wrote a little program, what exactly are you saying?

[hoss2006]

Hey project5k,
this is what I wrote for the timing pulley to see if it worked.

G0 Z-.015
G01 X.5 F10
G0 A.0625
G01 X0 F10
G0 A.125
G01 X.5 F10
G0 A.1875
G01 X0 F10
G0 A.25
G01 X.5 F10
G0 A.3125
G01 X0 F10
G0 A.375
G01 X.5 F10
G0 A.4375
G01 X0 F10
G0 A.50
G01 X.5 F10
G0 A.5625
G01 X0 F10
G0 A.625
G01 X.5 F10
G0 A.6875
G01 X0 F10
G0 A.75
G01 X.5 F10
G0 A.8125
G01 X0 F10
G0 A.875
G01 X.5 F10
G0 A.9375
G01 X0 F10
G0 A1.

I just positioned the endmill where i wanted it to start and pushed Go.
it made one cycle around the pulley.
i rewound the program, re zeroed mach 3 and hit go again for another pass.
For a finished program i'd set the z depth to say -.075 and use Z inhibit for multiple passes down to it.
Add all the cancel comp etc codes on the first line too to be safe.
I'm learning to write the code instead of relying on CAM too much for simple stuff.
But a nice CAM program is a must for most jobs.
Get grief from the guys at work that run CNC, they do it all with Notepad.
Hoss

[hoss2006]

Thought of a way to get the 4th axis to cut threads and tried it out this morning.
Seemed to work just fine.
Wrote another little program to cut 1 in of threads at 5 tpi.
Used a 1/8 endmill so it made square looking threads.
Wonder if I could find an endmill with a 60 deg tip?
Made another program to cut 16 tpi but used the lathe attachment tool holder.
it worked but left them a little rough. A sharper tool would work better than the carbide bit I bet.
I'll play around some more later, the parts for the table expansions are coming tues.
I should get a maid so that I could spend more than a few hours on Sat and Sun playing around with the mill. I hate housework.
this is the 5tpi test program

G0 X0 Y0
G01 Z-.01 F25
G01 X-1.0 A5.0
G0 Z0
X0 Y0
G01 Z-.02 F25
G01 X-1.0 A10.0
G0 Z0
X0 Y0
G01 Z-.03 F25
G01 X-1.0 A15.0
G0 Z0
X0 Y0
G01 Z-.04 F25
G01 X-1.0 A20.0
G0 Z0
X0 Y0
G01 Z-.05 F25
G01 X-1.0 A25.0
G0 Z0
X0 Y0
G01 Z-.06 F25
G01 X-1.0 A30.0
G0 Z0
X0 Y0
G01 Z-.07 F25
G01 X-1.0 A35.0
G0 Z0
X0 Y0
G01 Z-.08 F25
G01 X-1.0 A40.0
G0 Z0
X0 Y0
M30
I'll have more videos of the thread cutting at Youtube shortly.
http://www.youtube.com/hossmachine
Later hoss

[project5k]

ok, so let me understand, when you did the 16tpi, you used a basically stationary lathe bit mounted on the head of the mill, and had a stepper motor turning the part through the lathe chuck deal that you made, so that it would know exactly where the part was in its rotation as it cut... ok, so how fast was the part turning when it was cutting? i can just see the part spinning and the head moving to the left as it spins, well i guess the table was really moving to the right, but its all relative...

I'm really not trying to be an a$$, i'm just so inexperienced, i'm trying to make sure i have my fat little head wrapped around the process... cause i just know that this is something that i'm gonna wanna do, so the more i learn now, before my mill is ready, the better off i'll be when i go to set it up, and try this stuff...

[hoss2006]

project5k,
I'd have to use my tach on lathe to see the RPM but it's really low,
maybe 25 rpm. I have the motor tuned to 40 ipm for rapids in mach 3
but it would probably go faster than that, we'll see. the faster it goes the better. Lets see 25 ipm and I have the A Axis set so 1.0 in = 1 rev so 25 rpm.
could go 40 rpm. More playing is necessary.
that picture makes it look like it's going fast but it's a new camera
i'll have to check the shutter speed.
hoss

[cyclestart]

it worked but left them a little rough. A sharper tool would work better than the carbide bit I bet.

Wonder if a tailstock would help also?

I should get a maid so that I could spend more than a few hours on Sat and Sun playing around with the mill. I hate housework.

Make me some ballscrew mounts and I'll do the housework. Even the windows! Hmm, on second thought gas is expensive these days.

Great videos, keep'em coming.

[digits]

I really love the pics of your screwcutting - very nice

I used my rotary table in anger today - one thing you might find useful is relative coordinates, which I believe can be switched on with a G91 and off with a G90. I had a shed load of z-moves and rotates to do, so I just cut and pasted the same A and Z moves into my script once I'd turned on the relative coords:

G91

G1 Z-0.5 F10
G1 A370 F600

G1 Z-0.5 F10
G1 A370 F600

...

G1 Z-0.5 F10
G1 A370 F600

G90

I chose 370 degrees so that the plunge point moved around the circumference of my bore.

What I can't seem to do correctly is a combined A-axis and Z-axis move - I want to drop by 0.5mm per-revolution, with an angular velocity of 600mm/min, but G1 Z-0.5 A370 F600 seems to send the A-axis into silly speeds, - does it try to move the Z at 600mm/min, and so then has to speed the A up accordingly?

[hoss2006]

What I can't seem to do correctly is a combined A-axis and Z-axis move - I want to drop by 0.5mm per-revolution, with an angular velocity of 600mm/min, but G1 Z-0.5 A370 F600 seems to send the A-axis into silly speeds, - does it try to move the Z at 600mm/min, and so then has to speed the A up accordingly?

Yes the F600 will make the Z on the same line move at that rate.
This code stuff is still new to me so I can't be a big help though, but you might
have to cut the feed down to something both axis can handle together.

[hoss2006]

Wonder if a tailstock would help also?

i'll finish it someday, stuck till I do.
These aren't good threads because i didn't compensate for the angle of the thread when i fed in each pass. i just went straight in instead of at 29.5 deg
like on a lathe.
I thought about that at work and figure i'd have to move the x-.0028 with each
z-.005 cut.
I'll play around with a threading cycle first. maybe the thread milling wizard might work. we'll see.
The 4th Axis is going to take alot of playing around with but it looks like it gonna be a lot of fun.

[Pres]

Yes the F600 will make the Z on the same line move at that rate.
This code stuff is still new to me so I can't be a big help though, but you might
have to cut the feed down to something both axis can handle together.

The controller has no knowledge of "feedrate" on a rotary axis.
Whenever a rotary movement is the biggest axis move you must manually calculate the feedrate.
A mill controller only "understands" linear moves in computing feedrate.
Pres
p.s. this is an age-old problem for mills with rotary axes.