A Axis Feed Rate (resolved)

All things related to the Centroid Acorn CNC Controller

Moderator: cnckeith

RGSparber
Posts: 150
Joined: Sat May 27, 2017 2:12 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 38D269533454-0111180523
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
Location: Phoenix, AZ
Contact:

A Axis Feed Rate (resolved)

Post by RGSparber »

Where do I look in the Centroid M-Series Operators Manual for an explanation of how feed rate is interpreted when I move in the XA "plane" (linear and angular motion)?

For example, if I execute G01 F5 A40 X4 in order to rotate the A axis 40 degrees while moving to 4" at a feed rate of 5, what will happen? Is there a secondary screen to define the diameter of the stock being rotated? Does the feed rate only apply to linear motion?

I did a search with "feed rate" and couldn't find anything that applied.

Thanks,

Rick
RGSparber
Posts: 150
Joined: Sat May 27, 2017 2:12 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 38D269533454-0111180523
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
Location: Phoenix, AZ
Contact:

Re: A Axis Feed Rate

Post by RGSparber »

At http://www.cncsnw.com/4thHowTo.htm I found an equation that takes linear and angular movement plus desired feed rate and produces the value that goes next to the "F" on the G code line. My problem with this equation is that the numerator is adding inches squared to degrees squared. That can't be right. The denominator looks OK. There they convert degrees into inches before squaring it so add inches squared to inches squared. The ratio must be unitless for the equation to work but it is not.

My impression is that the Centroid software treats one degree of rotation as being equal to 1 inch as far as feed rate. For example F1 applied to linear motion Is 1 inch per minute but when applied to angular motion it is 1 degree per minute. Is that true?

Thanks,

Rick
RGSparber
Posts: 150
Joined: Sat May 27, 2017 2:12 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 38D269533454-0111180523
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
Location: Phoenix, AZ
Contact:

Re: A Axis Feed Rate

Post by RGSparber »

I found in the Mill user's manual, chapter 11:

F - Feedrate
The F command is used to set the cutting feedrate. The feedrate is expressed in units/minute. The programmed
feedrate may be modified by the feedrate override knob (2 - 200% for DC systems and 2 – 100% for AC systems).
The default feedrate is 3.0 units/minute. Units may be inches or millimeters.
Example:
G90 G1 X1.0 F50 ; linear mill to X1 at 50 units/minute

"Units may be inches or millimeters." So what about angular movements?

Rick
diycncscott

Re: A Axis Feed Rate

Post by diycncscott »

Rick,

It' much easier than calculating the rotary feedrate manually. Simply set parameter 2 to 8.

By default, rotary movements are in degrees/minute.

If you have an interpolated move that includes linear and rotary axes, the default feedrate is still specified in degrees/min. If you wish to specify moves that include rotary and linear axes, see parameter 2 in the manual.

To set it to slave the rotary feedrate to the linear feedrate, set it to 8.
For example (start point X0, A0):
G1 X10 A180 F10

The X axis will complete the move in 1 minute. The A axis will move at whatever rate it needs to in order to maintain interpolation with X. In this case 180 degrees/min. Keep in mind however that feedrates are modal so if you then command A0, it will again move at 180 degrees/min. If you wish to prevent this and have the modal value of the A axis feedrate remain at the feedrate programmed for last rotary only move commanded, set parameter 2 to 40 (32 + 8)
RGSparber
Posts: 150
Joined: Sat May 27, 2017 2:12 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 38D269533454-0111180523
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
Location: Phoenix, AZ
Contact:

Re: A Axis Feed Rate

Post by RGSparber »

diycncscott wrote: Fri Aug 18, 2017 7:05 am Rick,

It' much easier than calculating the rotary feedrate manually. Simply set parameter 2 to 8.

By default, rotary movements are in degrees/minute.

If you have an interpolated move that includes linear and rotary axes, the default feedrate is still specified in degrees/min. If you wish to specify moves that include rotary and linear axes, see parameter 2 in the manual.

To set it to slave the rotary feedrate to the linear feedrate, set it to 8.
For example (start point X0, A0):
G1 X10 A180 F10

The X axis will complete the move in 1 minute. The A axis will move at whatever rate it needs to in order to maintain interpolation with X. In this case 180 degrees/min. Keep in mind however that feedrates are modal so if you then command A0, it will again move at 180 degrees/min. If you wish to prevent this and have the modal value of the A axis feedrate remain at the feedrate programmed for last rotary only move commanded, set parameter 2 to 40 (32 + 8)
Thank you so much for the detailed and logical answer. One minor point. You wrote G1 X10 A180 F10 but then said the move takes 1 minute. did you mean to write F1.0?

After I fully understand what you wrote, I will write it up, with proper credit to you, and post the link in this thread.

Thanks!

Rick
diycncscott

Re: A Axis Feed Rate

Post by diycncscott »

No. A 10" move at 10"/min (F10) takes 1 minute to complete.
RGSparber
Posts: 150
Joined: Sat May 27, 2017 2:12 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 38D269533454-0111180523
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
Location: Phoenix, AZ
Contact:

Re: A Axis Feed Rate

Post by RGSparber »

diycncscott wrote: Fri Aug 18, 2017 12:50 pm No. A 10" move at 10"/min (F10) takes 1 minute to complete.
Of course. Not sure why I missed that.

So given G1 X10 A180 F10, my X axis feed rate is 10 IPM. At 10" and 180°, this is a pitch of 20". If my equation is right, the feed rate experienced by the cutter will depend on the diameter of the stock. If the diameter is 2", I calculate a feed rate as seen by the cutter to be 10.5 IPM. Not much difference. This makes sense to me because most of the motion is along the X axis.

But if I had G1 X10 A7200 F10, with a 2" diameter, the pitch would be 0.5" and the feed rate seen by the cutter is 126 IPM. Now most of the motion is due to A rotation. In general, the larger the diameter and the smaller the pitch, the higher the feed rate seen by the cutter relative to the X motion.

Does this make sense to you?

Thanks for your help,

Rick
diycncscott

Re: A Axis Feed Rate

Post by diycncscott »

Rick,

Yes, you are correct. A 2" diameter circle has a circumference of 6.283185... (Pi * D). You can think of the total distance traveled as a rolled up rectangle so just plug your number into the Pythagoras theorem. A^+B^2 = C^2 or C= square root of 10^2 + 3.14159265....^2 = ~10.48187....
RGSparber
Posts: 150
Joined: Sat May 27, 2017 2:12 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 38D269533454-0111180523
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
Location: Phoenix, AZ
Contact:

Re: A Axis Feed Rate

Post by RGSparber »

Thanks for the confirmation. I have published the article on my web site and can put a copy on this site too. How do I do that?

Questions, comments, and corrections welcome.

http://rick.sparber.org/HCAX.pdf

Rick
cnckeith
Posts: 7164
Joined: Wed Mar 03, 2010 4:23 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: Yes
Oak CNC controller: Yes
CNC Control System Serial Number: none
DC3IOB: Yes
CNC11: Yes
CPU10 or CPU7: Yes
Contact:

Re: A Axis Feed Rate

Post by cnckeith »

Rick,
Hello.
Very nice.
fyi..you can also use Centroid's conversational programming software "Intercon" to program a 4th axis helix as well.
helix intercon.JPG
here is the G code generated by intercon for the above helical move in W and X
; ICN_PATH = c:\MillDemo\ncfiles\helix.icn
; --- Header ---
N0001 ; CNC code generated by Intercon v3.15 Dev Test, Rev 10
; Description:
; Programmer: jk
; Date: 22-Aug-2017
M25 G49 ; Goto Z home, cancel tool length offset
G17 G40 ; Setup for XY plane, no cutter comp
G20 ; inch measurements
G80 ; Cancel canned cycles
G90 ; absolute positioning
G98 ; canned cycle initial point return
; --- Rapid Traverse ---
N0002 G0 X0.0 Y0.0 Z0.0
; --- Line ---
N0003 G1 X-4.0 Y0.0 Z0.0 W1440.0 F80.0
; --- End of Program ---
N0004 G49 H0 M25
G40 ; Cutter Comp Off
M5 ; Spindle Off
M9 ; Coolant Off
G80 ; Cancel canned cycles
M30 ; End of program
Need support? READ THIS POST first. http://centroidcncforum.com/viewtopic.php?f=60&t=1043
All Acorn Documentation is located here: viewtopic.php?f=60&t=3397
Answers to common questions: viewforum.php?f=63
and here viewforum.php?f=61
Gear we use but don't sell. https://www.centroidcnc.com/centroid_di ... _gear.html
Post Reply