Hello Guest it is July 14, 2020, 07:52:35 PM

Author Topic: What Steps/ Units Settings for Z-axis (Quill) of CNC Retrofitted Radial Machine?  (Read 20878 times)

0 Members and 1 Guest are viewing this topic.

Offline RICH

*
  • *
  •  7,411 7,411
    • View Profile
KHALID,
Try running this file. It mimics the pump vanes and there are a number of
Z travels and goes about cutting the profile such that moves are made to different points
on the profile. The file starts at x & y =0  and returns back to 0,0 with the Z retracted to 1" above Z=0.

 Note that the feedrate is set at 40 ( LINE N100 ). Change it to INCREASING different values, say 2,4,8,10,20 and see what happens.
You may want to try it in CV and exact stop mode.

You may want to put a pointed object in the quill or use your pen and trace it out on paper.

I believe it will tell something.............

RICH

Offline khalid

*
  •  213 213
    • View Profile
    • My Wood carving
Hi RICH,Thanks for coming back and the file... I just watched your file and the code contains IJ parameters ..  so should have to change to IJ mode in Mach3.

I will defintly try it tomorrow and show you the results:)

Offline RICH

*
  • *
  •  7,411 7,411
    • View Profile
The G91.1 in the test file  is incremental IJK mode.
I don't know what your defaults are so you may want to add the G64 on a line.

Yes the code is made up of arcs instead of your posted file which were all line segments. The arcs would give a cleaner
finish pass for the vanes.

Rich

Offline khalid

*
  •  213 213
    • View Profile
    • My Wood carving
Hmm...Thanks RICH:).. I will definetly try it tomorrow and will show whats comeup with the setup:)

Offline khalid

*
  •  213 213
    • View Profile
    • My Wood carving
Hi RICH... I modified my PEN and it is working right now:) Attached picture is the result of the Gcode you provided...

Offline RICH

*
  • *
  •  7,411 7,411
    • View Profile
Looks good, the backlash seems to be working ok on the Z otherwise you would have dug into the paper with the pen and tracking ok in the
x & y.
What F did you run it at?
Did you try cv and exact stop?
After running the program did you bring the Z down and see if it returned to the starting point? If it ran well at say one F, just double the feedrate and
 run it again since you returned  to the starting point, see if it tracks the same line and returns to the center starting point. At some F she will skip
and then you will know the max velocity you can run at. Then limit it to say 50 or 60 % of ( the 50 to 40 % reduction allows for torque required for cutting).

Then you can use a end mill to do some cutting in some scrap piece experimenting with some cut depths.

After playing around you will have some level of confidence on the F /  max velocity you should be using along with anticipated accuracy.

---------------------
Your original program had short straight line segments instead of the arcs.That can create a problem for YOU depending on the accel values
and mode you are running ( cv or exact stop ).
Let me comment that in your program you clean out the bulk of the material in the first area and then finish the first vane of the impeller , then
 the others go on to profile the vanes only. Do as you wish, but, i would have cleared out all the bulk and then profiled the impellers.

Like said before, wood is different than cutting metal, so fool around to gain experince with YOUR machine.

"SPEED WILL COME UNBIDDEN ONCE ACCURACY IS ATTAINED"  ;)

RICH

Offline khalid

*
  •  213 213
    • View Profile
    • My Wood carving
Looks good, the backlash seems to be working ok on the Z otherwise you would have dug into the paper with the pen and tracking ok in the
x & y.
What F did you run it at?
Did you try cv and exact stop?

Actually i modified the PEN a little .. The pen comes with spring and on One click the point comes out and on the other click the tip get inside.. I modified it a little and it worked very fine as you have seen in the picture..

I ran the Gcode with F10 and i used CV mode On...
After running the program did you bring the Z down and see if it returned to the starting point? If it ran well at say one F, just double the feedrate and
 run it again since you returned  to the starting point, see if it tracks the same line and returns to the center starting point. At some F she will skip
and then you will know the max velocity you can run at. Then limit it to say 50 or 60 % of ( the 50 to 40 % reduction allows for torque required for cutting).
Yes the Program return to its exact start point..and the Z when commanded to go to zero, it exactly went to the zero location... I imported yours Gcode into NCPlot and exported in DXF... I open the DXF in AutoCAD and measured some dimensions and compared it with the pen-tracing... I was within 0.07mm range.. Amazing:)... As it was on the Paper so measurement was not easy by Vernier calipre;)

I just tried if with F10, tomorrow i will increase the velocity and will show you some more results:)... Lets say F10 is my maximum velocity then i have to keep my rapid F5 and keep the cutting 4IPM....Am I right.. My Stepper motors are for 80Volts rating with 4.2Amp per phase..Currently i am only supplying 36Volts DC.. I have connections of 48Volts and 60Volts too.. I will try increasing the voltage...

It is now clear that My Y-axis i.e. the bottom carriage , loosing steps.. This is because it carries the load of X-axis carriage+Workpiece load+Cutting forces.. It is boxway design so having frictional forces too (although i have appled Oil too)...






Then you can use a end mill to do some cutting in some scrap piece experimenting with some cut depths.

After playing around you will have some level of confidence on the F /  max velocity you should be using along with anticipated accuracy.
I will sure do so.. I am planning to use 1mm DOC for Aluminum... My Z-axis has some play, in the impeller case the Gcode was 2mm per pass and the first pass of the impeller was 3.5mm.. That was too much for the cutter..... so i will use shallow cut in future...

---------------------


Your original program had short straight line segments instead of the arcs.That can create a problem for YOU depending on the accel values
and mode you are running ( cv or exact stop ).

Yes, today i figured out how to output the gcode in G02/G03 IJK mode.. so in future i will make my Gcode more clean.. I am also planning to Use EXACT STOP MODE for milling... I hope that for better usage of Backlash compensation i should not use CONSTANT VELOCITY MODE...


Let me comment that in your program you clean out the bulk of the material in the first area and then finish the first vane of the impeller , then
 the others go on to profile the vanes only. Do as you wish, but, i would have cleared out all the bulk and then profiled the impellers.

Like said before, wood is different than cutting metal, so fool around to gain experince with YOUR machine.

"SPEED WILL COME UNBIDDEN ONCE ACCURACY IS ATTAINED"  ;)

RICH
The Gcode for the above impeller was made in ARTCAM.. and I know artcam is good for wax/wood but not for metal... I will use VisualMill for my next Gcode generation projects... I will follow your advice and will post you some good results..

Thanks for being with me and helping me:)

ONE QUESTION:
If my motors do not loose steps.. Then will the Backlash compensation will be OKAY for heavy Cuts?.. I read somewhere that Backlash compensation do not work for heavy cut.. Please enlighten me:)

Offline RICH

*
  • *
  •  7,411 7,411
    • View Profile
You don't want to skip steps for rapid moves or during actual cutting. If through eperience on many files you find that you can rapid
at 10 IPM and nothing goes wrong, then maybe try 20. if you skip then try 12 and see what happens. I don't know if 10 is near say the limit
for your machine ( there are programs that can be used to evaluate the adequacy of the system for a given rapid ). It's more than just the velocity
as accel / decel is important also. You just want some headroom / be at a combination of velocity / accel setting that you can be confident with.
If your at the edge of settings, say your machine is not lubricated well, then addtional additional stepper torque will be required at that setting and
thus you could skip, so you reduce the settings.

Now when you start cutting metal, additional torque is required, so you know you want to be below what the confortable rapid is. 
There is a big difference between Al, steel, cast iron, etc. SO maybe you find that all is well with Al but you need to adjust for the harder to machine metals.


Best point to be made to you is, the axis settings should be such that the axis can be run at with max POWER (  =SPEED x TORQUE) relative to the stepper motor curve.
Of course consider F and spindle speed ......etc when doing something.

---------------------
Carefull with the backlash, with small diameter end mills you can break them in a heart beat. Rule of thumb is max depth of cut  less than 1/2 dia of mill.
BC works fine for me for whatever i have done. The "heavy cutter" folks  can chime in with their experience on any problems.
 

My 50-50-50 rule which you may want to consider.
50% - The max velocity is 50% of where your steppers will start to skip
50% - Set the shuttle Wheel setting in configuration to .0050  to .050 ( .5 too slow )
50% - Backlash speed
This is a good starting point and refine upward, but always leave say 30% headroom

RICH

Offline khalid

*
  •  213 213
    • View Profile
    • My Wood carving
Hi Rich,
I have checked the Gib Tighteness... Following were my observations:

1- The Y-axis Ball screw has 3inch dia pully installed.. I removed the belt and rotated the pully with One thumb and 3-Fingers... I was feeling the force of moving the Slide... The Screw has some spring action inside.. The wheel is turned first upto a limit with the screw and then screw nut takes the load and further after quarter turn the slide was moving...

I then adjusted the Taper wedge.. and now my Y-slide is moved with only two fingers and not enough force... For comparasion i would say i have reduced 50% force for movind the slide by loosening the taper wedge... I also checked the slope and it was un-noticable... The slide is very very Free now

2- The same procedure was adopted for my X_slide and it is also improved 50% from the previous...

Today i recalibrated X and Y axes as i have loosen the gibs.. I Did some real drilling on the SS-316 tube sheet of one of the exchanger we are fabricating... You can see the centre drills and two 8mm deep drills... The OTL (Outer Tube limit)is under 0.03mm... I also measure 14holes across and the commulative length is under 0.02mm...Now, I can drill SS-316 upto 33mm deep ...

The slides are very free moving after loosing the taper wedges..It seems that i have installed the linear rails
I am planning to make the new spindle with AISI 4140...Today I have hardened 03 different cylindrical pieces( dia: 1inch, length 1.5") of AISI 4140..
Each piece was heated to 850C and then one piece was Oil Quenched, One was Normal water Quench whereas the last one was quenched in the chilled water...
I have observed the longitudinal crack in the normal water quenched workpiece...

Following are the hardness results of 4140 test pieces..

A) Oil Quenched: 38.8HRC
B) Normal Water (Amb. temp): 54.1 HRC
C) Chilled Water: 49.8HRC

I cut half the option B, material and again taken the readings at the centre. I got 50HRC...That is excellent for spindle... For a good spindle the hardness must be in the range of 50~57HRC..

The Spindle is roughly machined out of AISI4140... I am going to Quench it on monday..

I am thankful to you for helping me...

Offline RICH

*
  • *
  •  7,411 7,411
    • View Profile
Khalid,
Happy your happy with the adjustments.
Nothing wrong with feel, i use a torque gauge to get values. Here is a link to my anal aproach
on a small lathe.
http://www.machsupport.com/forum/index.php/topic,12484.msg81868.html#msg81868
FWIW,
RICH