Welcome, Guest. Please login or register.
Did you miss your activation email?
December 21, 2014, 10:06:03 AM

Login with username, password and session length
Search:     Advanced search
* Home Help Search Calendar Links Login Register
+  Machsupport Forum
|-+  Mach Discussion
| |-+  General Mach Discussion
| | |-+  4th axis
Pages: 1 2 »   Go Down
Print
Author Topic: 4th axis  (Read 3090 times)
0 Members and 1 Guest are viewing this topic.
bfairey
Active Member

Offline Offline

Posts: 40


View Profile
« on: August 01, 2009, 02:32:34 PM »

How do I setup and program my 4th (rotary) axis?
Brian.
Logged
olf20
Active Member

Offline Offline

Posts: 204


View Profile
« Reply #1 on: August 01, 2009, 05:53:40 PM »

Hi Brian, here is a link to a thread. Lots of information.

http://www.machsupport.com/forum/index.php/topic,5281.0.html

Reply 14 has details which I use.

There are several ways to do this depending on your particular machine,
and needs.

Hope this helps!
olf20 / Bob
Logged

Mach3, Atlas Knee Mill, 4th Axis, VcarvePro
Been Heating with corn since 1998
Chip
Global Moderator
*
Offline Offline

Posts: 2,058

Gainesville Florida USA



View Profile
« Reply #2 on: August 01, 2009, 07:41:50 PM »

Hi, Brian

Pic's below should get you started, There are a couple of ways to set up Steps Per, Hears 1 way, Determine the number of steps it takes to turn 1 complete turn and divide it by 360, That will give you steps per "Deg.", Enter it as your Steps per value in motor tuning.

Example: Stepper motor 200 steps X 10 micro step driver = 2,000 X 72 turn rot. table = 144,000 steps for 1 turn / 360 = 400 steps per Deg.

It all sounds confusing, Give it a shot and ask more Question's as needed.

Chip


* AAAA.jpg (46.66 KB, 518x385 - viewed 265 times.)

* AAAB.jpg (100.35 KB, 712x466 - viewed 272 times.)

* Chip_004 Aug. 01 17.00.jpg (134.74 KB, 1258x401 - viewed 271 times.)
* A-Tesr Rot g91 first A.tap (0.19 KB - downloaded 118 times.)
Logged
Cartierusm
Active Member

Offline Offline

Posts: 113


View Profile
« Reply #3 on: August 06, 2009, 06:11:03 PM »

Howdy, I just setup my 4th axis today and I had a couple of questions.

Chip, on the Settings Tab that your pictured is that where you put in the diameter of the stock you're working with? If so how does it know if you are using a complex piece that's been made on a lathe with lots of curves that you want to engrave? For your info I think I'll be using 4th Axis option in my RhinoCam so maybe that takes care of that?

Also I'm a bit confused on the calculation, well not confused I understand them but confused on the operation. I have a pulley system as I adapted a spare Lathe Head, just hooked up some timing pulleys and a stepper. I used an online pulley calculator to detemine I have a .416 ratio, which means that it takes 2.4038 turns of my stepper to turn the 4th axis 1 revolution. Now if I go by your calculations I take that and times that by my 2000 steps per revolution of my stepper (200x10microsteps) and then divide by 360, I get 13.354. Now if I put that into my Motor Tuning and then jog it goes real slow, but if I go the full amount 2.4038*2000=4807.6 then it moves at a good rate. Is it supposed to turn slow?

Last question on the first picture above, does that need to be checked for all situations or is that if you are substituting an axis Letter in your G-code? I'm going to be using RhinoCam which has 4th axis support so not sure if it will output it as "A"?

Thanks.
Logged
olf20
Active Member

Offline Offline

Posts: 204


View Profile
« Reply #4 on: August 06, 2009, 07:10:29 PM »

Hi Brian, glad to hear you got your system running.

If you have your system setup as A being your rotary you can only use it as rotary / degrees,
If I understand it correctly.

Here is a quote from Art;
 You have it right. You cannot do arcs other than in the XY plane, XZ plane or YZ plane. There is no conceptual plane for
a rotary axis. The checkbox for linear/angular only tells an axis not to convert when switching from mm to inch, other than that it
has no purpose. A, B and C are always rotary axis.. So using an IJ with an A axis is an error in syntax, though still legal, the missing Y in this case would simply be interpreted as the current Y location, and the A would just be a linearised motion on that axis during the movement of the XY
in the XY plane arc.


As I do not have any software that supports 4Th axis / A I chose to have my rotary to be driven by my Y axis.
This is where the post that I referred to comes into play.
I'm sorry if I'm not explaining this very well. I'm somewhat new to it all but have got great result with mine so far.

olf20 / Bob
« Last Edit: August 06, 2009, 07:12:01 PM by olf20 » Logged

Mach3, Atlas Knee Mill, 4th Axis, VcarvePro
Been Heating with corn since 1998
Cartierusm
Active Member

Offline Offline

Posts: 113


View Profile
« Reply #5 on: August 06, 2009, 07:28:46 PM »

I just tried running a file I made in RhinoCam and it moves really slow, I mean it would take 20 hours for it to do anything, so there is something or some setting wrong. Here are my XML and the Gcode.

* Mill Pref2.xml (98.31 KB - downloaded 83 times.)
* 4th Axis Test 0.txt (36.99 KB - downloaded 125 times.)
Logged
Greolt
Global Moderator
*
Offline Offline

Posts: 933


View Profile
« Reply #6 on: August 06, 2009, 08:50:52 PM »

I ran your code.  5ipm is kinda slow anyway but I am guessing that was intentional.

Play around with the "Rotation Diameters" on the settings page (which I think should read "Rotation Radius")

Mach tries to adjust feedrates for different Z DRO readings.

Every time I think I have a good grasp of what it does there, something comes up to say I have not.  Cheesy

What I think it does, is take the Z DRO value and add it to the Diameter (radius) setting and adjust the A axis feed rate to suit that total.

So if you have Z zero at the centre of rotation then set the "Rotation Diameter" to near zero.  (not zero or it will not work)

And if your Z zero is at the cutting radius then set that as the "Rotation Diameter"

I am very ready to be set straight if this interpretation is incorrect.  Cheesy

Greg
Logged
Cartierusm
Active Member

Offline Offline

Posts: 113


View Profile
« Reply #7 on: August 06, 2009, 09:23:06 PM »

Yeah thanks, that confused me even more LOL. I'll reread what you said. I was doing 5IPM because I was engraving with a fine bit.

So I have my parts center as the center so it should be going to like 1.2" up and cutting but it doesn't do much. I'll mess with the settings.
Logged
alenz
Active Member

Offline Offline

Posts: 137


View Profile
« Reply #8 on: August 06, 2009, 11:18:20 PM »

Yeah thanks, that confused me even more LOL. I'll reread what you said. I was doing 5IPM because I was engraving with a fine bit.

So I have my parts center as the center so it should be going to like 1.2" up and cutting but it doesn't do much. I'll mess with the settings.
Greg has you on the right track.  Here in a nutshell is what’s required.

In Config> General Config be sure ‘Rot 360 Rollover’ is NOT checked. (Your code uses both pos and neg A values).

In Config> ToolPath select the ‘X-axes’ button; check ‘A-Rotations Enabled’ and check ‘Use Diameter for Feedrate’.

On the Settings page you have a choice with the ‘Rotation Diameter’ DRO. Unfortunately due to a problem within Mach, neither is accurate, but in your case one is better than the other.

 If you enter 0.0001 in the DRO then Mach will read all Z values as a diameter and calculate the feed rate accordingly. Obviously, this is incorrect as the Z is actually a radius. The angular component of your X-A move will be off by a factor of 2. Probably not acceptable.

If you enter the Z value that is in the first block containing a Z then in this case (and in this case only) Mach will correctly use this value as a radius. However changes in Z will be incorrectly interpreted as a change in diameter thus creating another error. But this error is less and in fact wouldn’t even be noticeable if your Z clearance height were reduced. (Less change in Z; less error). Is there a reason that you need over an inch of Z clearance? (I normally use something more in the order of 0.050).

Another thing, your code uses only   G01 (no G00), although it does increase the feed from F5 to F20 for the rapids. You may find it more convenient to use G00 for the rapids and thus only have to set the Feed rate once at the beginning. Easier to make changes.

 Is it just me, or are you engraving a mirror image?

Hope this helps,
Al
Logged
Cartierusm
Active Member

Offline Offline

Posts: 113


View Profile
« Reply #9 on: August 07, 2009, 11:57:28 AM »

No I'm not engraving a mirror image, it's just my name on a round piece of stock. I don't need an inch of clearance, from the tutorial in RhinoCam it says to make the center of the round stock the center. Should I move my part in Rhino Down so the top facing the milling bit is Zero? I'd prefer that way so I can just do a touch off of Z for my Z-Zero.

What I don't understand is that rotational diameter, I don't have to understand it to use it, so I shouldn't put a value of .0001 in, but I should put in the value of the first Z block in my code. So if I set the top of my stock to zero with my bit and the first depth in my Gcode is .005, which is as deep as I'm going with my bit, then this will work?

Thanks.
Logged
Pages: 1 2 »   Go Up
Print
Jump to:  

Powered by MySQL Powered by PHP Powered by SMF 1.1.20 | SMF © 2013, Simple Machines Valid XHTML 1.0! Valid CSS!