# School Me - Cnc Circle Cutting Test. Mach3, Amoeba's For Circles.



## countryguy (May 9, 2015)

Hi gang. I'm new... I know that there is soooo much my Son (18 in a few weeks) and I do not really grasp yet. Following tips and docs all over from the web. The groups here are really great. On the shopmaster 3:1 Patriots- I have a 2010 w/ the x screw on the side of the saddle. I have done and learned a lot about Mach 3, steppers, and dial gauges, w/ DRO's glass scales, etc.. All that was fun and we needed to learn how to do it. We are trying to do a lot fast. Always a recipe for some trouble. Maybe... Maybe not. So below is my issue. I hope the fellow Patriot users here can offer some patient suggestions and ask me to go do this or that and report back. I really want to solve this... and my never-give uped'ness keeps me in the shop w/o stopping to ask Q's at times. 

Now, We're actually making things! I need to push a set bronze oilite sleeve brearing into a 1" x 1" x 6" block. I milled the block and the Tram seems Fair/Ok. not overly horrible. 
PROBLEM: I knew cutting the holes would be the "nag" item that sent me asking Q's and tearing into "Why" The Holes (pic below) are all Amoebas! Irregular and misshapen. 

A) I'm pretty sure I can still just press in the sleeves w/o much concern as long as I stay square. I have some 'wiggle room and it's nothing terribly precise. 
B) But what the hey' What can't I get this thing to cut a clean Circle? Or what can you suggest in order to get to a better circle mil.? Or is this a fools gold task? 

C) Pic: Cut w/ 1/4" two flute via GWizard settings, slowed way down to fine finish. 3200RPM and I think 10 or 12 ipm. Kept the tooth IPT right on anyway

D) Tried w/ BackLash on & Off. Ehhh so so better w/ BL on. Want to try screw mapping but I'm not sure of that yet. Reading up! Anyone think that would help map out the saddle shift? (see note E on this comment).

E) Back story: Upgraded lower end wound (not ground) screws w/ precision balls. Poked, played, tweaked Mach3 settings, DRO Calibrate, Dial indi's Finger Indi's, gibs, etc. We spent a NEWBIE month on it. We were really proud that when I move 1" - I get .9997 or 1.0001 regularly on the Jenix glass scales, the MAch3 DRO, and the Dail Indicator. That's in X and Y ..The but- The but is Backlash on X is still set to .0035. Y .001 and Z .001 and if not set, I'm off. And it's pretty cool to see that all work after all the efforts!!!   The side based X screw does lend to saddle sway. I can even see it so I'm leaning into that as job #1? But do not really know how to solve it yet. Maybe this is a known issue?  Maybe Not so much?   
F) Data gathering. Hmmm, Where to even start? I know . I know.... A night sleep for starters  Wiped out today. I ask a lot of Q's and our desire to learn is larger than our hours in the day. But what a fun adventure we're havin. 

G) Pic. 
H) YEah- PS- I went out and found a great SuperMax YMC 30 taper CNC mill in great shape. built 1985. I installed the Ajax Centroid kit myself and this thing is the 'B O M B'! Now that cuts holes just fine and very regular & repeatable thus far. ( I have not even done the 'fine adjustment' doc-set procedures yet). Thats the hole set on the left.


----------



## T Bredehoft (May 10, 2015)

Without hands-on I can only guess, but let's start looking for lead screw backlash.  The controller says turn left and the tool waits .005 before it turns, or something like that. This is a simplification, the tool doesn't move, the table does. But its still backlash.


----------



## RJSakowski (May 10, 2015)

Pocketing routines are not generally used for precision holes.  Use a boring head or drill and ream instead.


----------



## JimDawson (May 10, 2015)

I guess there is a couple of things that I would look at.  As Tom stated, the backlash is an issue, but I have seen Mach3 do this when I knew that there was zero lash in the system using preloaded double ball nuts.  The Mach3 backlash compensation does not work at all when cutting, only when making a position move, so there is a good chance that that is a problem.

I would start with the CAM program and make sure that it is creating a G2 or a G3 command rather converting circles to line segments.  I general, Mach3 does a pretty good job on larger circles and arc segments, but not so well on smaller circles.  Just the dwell of the tool  as the motor changes direction can be enough to cause the amoeba  shape.  You might try running the finish profile 2 or 3 times to see if that cleans up the circle, this might overcome the tool/system spring.


----------



## TomS (May 10, 2015)

T Bredehoft said:


> Without hands-on I can only guess, but let's start looking for lead screw backlash.  The controller says turn left and the tool waits .005 before it turns, or something like that. This is a simplification, the tool doesn't move, the table does. But its still backlash.



Maybe this is a good place and time to start a discussion on checking/measuring backlash and correcting it, or at least minimizing it.  The net has a lot of info on this subject but it's spread all over the place and it doesn't always apply to hobby CNC machines.  Would be nice to consolidate everyone's thoughts into one thread.

My 2 cents.

Thanks


----------



## T Bredehoft (May 10, 2015)

What cutter are you using?  If they are 3/8 holes, I'd try finishing them with a 1/8 four flute. or smaller if you have it.


----------



## countryguy (May 11, 2015)

Hi Eveyone,  
Thanks so much for the Reply.   Now I understand what the reamer is for.  Or and adjustable reamer to get a for cut home. I simply did not know that an area clear is not what ya would do here!  Thanks RJ.   
We are  on the road to mechanicsburg pa to pick up the heat treating muffle furnace. Wil be home in a few days.   Father son 
Road trip.     Anyone want a 17yr old. Lol.


----------



## RonGinger (May 13, 2015)

JimDawson said:


> The Mach3 backlash compensation does not work at all when cutting, only when making a position move, so there is a good chance that that is a problem.



This is not true- Mach3 makes a backlash adjustment anytime an axis changes direction, whether its making a rapid or feed rate move. It would be rather useless if it only adjusted in rapid moves.

I do not believe backlash compensation is useful. While the backlash is being corrected the table is unconstrained and the tool is likely to divot the work. Backlash elimination is what we need, not compensation.


----------



## JimDawson (May 13, 2015)

RonGinger said:


> This is not true- Mach3 makes a backlash adjustment anytime an axis changes direction, whether its making a rapid or feed rate move. It would be rather useless if it only adjusted in rapid moves.
> 
> I do not believe backlash compensation is useful. While the backlash is being corrected the table is unconstrained and the tool is likely to divot the work. Backlash elimination is what we need, not compensation.




Thank you for commenting Ron.  I was going by the following excerpt from the Mach3 manual.

_''5.6.3 Configure Backlash Mach3 will attempt to compensate for backlash in axis drive mechanisms by attempting to approach each required coordinate from the same direction. While this is useful in applications like drilling or boring, it cannot overcome problems with the machine in continuous cutting.''_

Maybe I am miss-interpreting what it says.

I do agree that the backlash should be eliminated mechanically.


----------



## countryguy (May 13, 2015)

Thanks.  I'm looking at some Surplus double-nut ball screws down the road possibly. 15-20mm  This 1/2" or 9mm or what ever offshore wrapped screw is just too wobbly and too small on this X setup.  
  If I am going to keep this Mill/Lathe I may as well improve it.    Will discuss on a post another time.  I'm just out of time for all these projects!   I guess It's fine as is for engraving and making some aluminum things.   But it's $4k I could use for something else too....  tough decision here.   I just do not have the time right now to eliminate the backlash.  I will setup a few things later when I get a slow day.     for noww THANKS Everyone for the posts and notes.   

Very helpful to know that any system, no matter High end or low end simply must be mechanically sound and with virtually no slop.     So many manuals and sites claim that they have C7 ball screws and this or that.  But nobody ever claims something like:  " *our mills go out the door w/ .0005 backlash or less on 4 axis.    *  I keep learning and you guy's keep posting!  

Gnite, JJ


----------



## countryguy (May 21, 2015)

Update:   Much Much better performance after quite a learning experience.  Here is the follow-up to help future Newbs possibly. 

Machine: Shopmaster Patriot.  Not the new Mill Turn. 
There were several helps on this noted below. 

Setup Backlash adjustments. Gage based Measurements, Motor tuning, and Mach3settings based on Hoss Vid. 
Mach3- Turn off CV on angles >90 degrees (Mach3, General config settings checkbox) Read to try in a few places. 
Fixing the Quill movement via a socket-screw into a machined quill slot. (biggest gains on this 1 fix for me).
Setting the tapered gib adjustments and experimenting with too loose, too tight- until best results.

All circles are right in there now! Very close (.001 / .002 ) from circle to circle. And .001 to .002 in 2 measurements 90' apart on circle. Ran groups of three circles 3 times.  What seems really cool now is that Mach3 and the glass DRO's are displaying tens to a thou difference.  Fluke or finally dialed in-  Time will tell.  But cool to see. 

Learned a Lot! Experiment, learn, repeat.   Man this stuff is not for the impatient that is for sure. 

CGout.


----------



## JimDawson (May 21, 2015)

Happy to hear it's better.  Patients pays off.


----------



## Firestopper (Jun 7, 2015)

Glad to read you've figured it out. 
I'm running Mach 3 on a ten year old plasma table and under "configurations" (top bar menu ) allows for calibrations inputs. Not sure if your version of Mach is similar, but I was able to recently recalibrate my steppers after timing/drive belt replacement. 
Sorry for the late reply, but I've been off line lately.
As others have mentioned, critical holes require boring and fine finish cutting. 
I need to start over on Mach some time in the near future as I'm still running Windows XP.

Glad to read you and your son spend time in the shop together.


----------



## astjp2 (Jun 18, 2015)

Cut a circle, triangle, square then compare them to the program.  this is what we do at work.  Checks that both X&Y motors run consistent.  I would do a 2" of each.  Tim


----------



## countryguy (Jun 19, 2015)

Hey Firestopper-  Just noticed your Pic on the Avatar.  WOW! That is a clean looking shop.  Very nice indeed!   
CG. 



firestopper said:


> Glad to read you've figured it out.
> I'm running Mach 3 on a ten year old plasma table and under "configurations" (top bar menu ) allows for calibrations inputs. Not sure if your version of Mach is similar, but I was able to recently recalibrate my steppers after timing/drive belt replacement.
> Sorry for the late reply, but I've been off line lately.
> As others have mentioned, critical holes require boring and fine finish cutting.
> ...


----------



## Firestopper (Jun 19, 2015)

Thank you CG, 

I finally built my dream shop. Keeping it clean is a work out haha, but worth it.


----------

