Re: [Emc-users] Rotary axis usage

2019-07-24 Thread Chris Albertson 
On Mon, Jul 22, 2019 at 12:07 PM John Dammeyer 
wrote:

>
> So how is this solved?   How would the A axis know the diameter and be
> able to translate that a request of F14.7 should really be F360 when Z is
> being moved at the same time?  Odds are I've configured the CAM software
> wrong but if I was going to just manually write some G-Code that involved
> simultaneous motion what would I do?


The math is not hard.  Assume you are tracking the position of X,Y,Z.SO
the cutter is at (x, y, z).  Assume the A axis is parallel to the X axis
and interectest the YZ plan at (Ya, Za)

The distance fromt cutter to the A axis is just the pythagoriam formula  =
square root( (y-Ya)^2 + (z-Za)^2 )
Then you always divide the roation rate by the above distance and you get a
constant cut rate.  But (x, y, z) constantly changes you you need to
re-compute the distance  continously before every g-code command.  Good
thing you have a computer.  I'd hate to have to write 4-axis code by hand.

The above might by done by a g-code interpeter or the CAM software or a
human coder.   It gets slightly harder if the rotation axis is not parallel
to either X, Y or Z axis. and even worse when three or four rotary tale are
stacked as in say a robot shoulder joint


-- 

Chris Albertson
Redondo Beach, California

___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Rotary axis usage

2019-07-23 Thread John Dammeyer 
I've done some more work testing the G93 with LinuxCNC after MecSoft laid out 
how they do the calculations.

Fundamentally, as has been stated before, the A axis is rotary and done in 
degrees.  However, the MecSoft code still treats the A axis as if it moved a 
physical distance.

Some simple tests have demonstrated this comparing a move of 5" on the X axis 
to an A Rotary axis move of 5" around the circumference of a 0.7958 Radius 
cylinder (360 degrees)

If the G-code is 
G93 G1 X5 F6 it takes 10 seconds to move the 5"
G93 G1 A5 F6 doesn't come close to moving 5"  Only 5 degrees.

If we assume the Z axis is set at -0.7958" then we'd set A to 360 degrees which 
is 5" worth of circumference.
G93 G1 A360 F6 and it also takes 10 seconds.  In fact if we move both at the 
same time
G93 G1 X5 A360 F6 they both finish at exactly the same time and both have moved 
the correct distance.

More complicated moves with multiple axis or Z changing will require some 
interesting math but it has to be done in the CAM software.

John Dammeyer




___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Rotary axis usage

2019-07-22 Thread John Dammeyer 
Yes.  MecSoft showed me how to set that up but I'm not impressed so far.I 
used the application from the link that Martin posted and compared the results. 
 First the AlibreCAM (MecSoft) file used G1 and the Fxx values were as a result 
very slow.   And F8.9 for a 3 degree A axis move still takes about 6 seconds.  
(1/8.9 * 60 = seconds for the move).

Change that G1 to a G0 and it speeds up.The program Martin linked doesn't 
accept the G-Code with G93 already installed.  So it has to be created without 
G93.  Then it also complained about the G1 and installed a G0 to set the 
speeds.   Speeds were now more like 1800 degrees/minute for a 3 degree turn of 
the axis.

So probably need to come up with a benchmark G-code set of lines that can then 
time how long it takes the rotary axis to move given that I might want a 
cutting speed of 12 IPM to avoid damaging the tool bit or the work.

John



> -Original Message-
> From: Greg Bentzinger via Emc-users [mailto:emc-
> us...@lists.sourceforge.net]
> Sent: July-22-19 7:30 PM
> To: emc-users@lists.sourceforge.net
> Cc: Greg Bentzinger
> Subject: Re: [Emc-users] Rotary axis usage
> 
> [Greg]
> BTW MecSoft added the Inverse time mode option to the AlibreCAM,
> RhinoCAM, and VisualMill plug in for SolidWorks.
> Once I get my Hurco Conversion functional I intend to do a series of
> LinuxCNC post processor files for the Mecsoft CAM engine.
> [/Greg]
> 
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Rotary axis usage

2019-07-22 Thread Greg Bentzinger via Emc-users 
[Greg]
BTW MecSoft added the Inverse time mode option to the AlibreCAM, RhinoCAM, and 
VisualMill plug in for SolidWorks.
Once I get my Hurco Conversion functional I intend to do a series of LinuxCNC 
post processor files for the Mecsoft CAM engine.
[/Greg]

___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Rotary axis usage

2019-07-22 Thread Gene Heskett 
On Monday 22 July 2019 15:21:50 Martin Dobbins wrote:

> Real fast reply John, but does this video help?
>
> https://www.youtube.com/watch?v=d0ffiCekhpE
>
> Martin
>
> 
> From: John Dammeyer 
> Sent: Monday, July 22, 2019 12:06 PM
> To: 'Enhanced Machine Controller (EMC)'
>  Subject: [Emc-users] Rotary axis
> usage
>
> I've run into a situation with the CAM file generated by MECSOFT
> AlibreCAM appears to have a problem.  I've asked this on the support
> group for AlibreCAM but I think it's a more general question involving
> simultaneous 4 axis milling where I write the G-Code myself.
>
>
> N1 G17 G20 G40 G90
> (4th Axis Create Cylinder/Round)
> N2 T2 M06
> N3 S2 M3
> N4 G0 X-2.2788 Y0. Z1.664 A46.8 F0.
> N5 G1 Z1.45 A46.8 F11.
> N6 X-2.4983 Z1.4113 A46.8
> N7 X-2.5389 Z1.404 A46.3
> N8 Z1.4 A45.
> N9 X-2.5388 A43.7 F14.7
> N10 X-2.4959 A43.2
> N11 X-0.0018 A43.2
>
>
> Effectively the feed rate on the X,Y and Z is 11 IPM or 14.7 IPM. But
> the rotary axis is angular under LinuxCNC and measured in degrees per
> minute. I believe that makes sense because the diameter of the part
> being rotated determines the actual feed rate. So if the circumference
> was 14.7" and the cutting speed is set at 14.7 IPM then the rotary
> axis should turn 360 degrees per minute.
>
> But as shown in line N9 we have simultaneous motion on X and A but at
> F14.7.
>
> Clearly if the diameter was such that the circumference was 29.4" then
> the feed rate of the A axis would have to be half or 180
> degrees/minute.
>
> Running the G-Code above sees the Z or X axis moving at the expected
> speed.  Watching paint dry is more interesting than watching the A
> axis turn.  But if I just do a G1 A360 F360 the motion of the A axis
> at 4.68 diameter  appears to be about the same speed  as the X or Z
> horizontally.  It also takes exactly 1 minute to move 360 degrees at
> 360 degrees/minute.
>
> So how is this solved?   How would the A axis know the diameter and be
> able to translate that a request of F14.7 should really be F360 when Z
> is being moved at the same time?  Odds are I've configured the CAM
> software wrong but if I was going to just manually write some G-Code
> that involved simultaneous motion what would I do?
>
> The AXIS display shows 14.7 for speed.  The Z is known.  Is there
> something missing so that the A axis actually gets a much faster rate?
>
> Thanks
> John

Thats purty. download the zip file by clicking on the MORE button below 
the video.  Otherwise  the dl link is hidden.

Cheers, Gene Heskett
-- 
"There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order."
-Ed Howdershelt (Author)
If we desire respect for the law, we must first make the law respectable.
 - Louis D. Brandeis
Genes Web page <http://geneslinuxbox.net:6309/gene>


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Rotary axis usage

2019-07-22 Thread Gene Heskett 
On Monday 22 July 2019 13:06:34 John Dammeyer wrote:

> I've run into a situation with the CAM file generated by MECSOFT
> AlibreCAM appears to have a problem.  I've asked this on the support
> group for AlibreCAM but I think it's a more general question involving
> simultaneous 4 axis milling where I write the G-Code myself.
>
>
> N1 G17 G20 G40 G90
> (4th Axis Create Cylinder/Round)
> N2 T2 M06
> N3 S2 M3
> N4 G0 X-2.2788 Y0. Z1.664 A46.8 F0.
> N5 G1 Z1.45 A46.8 F11.
> N6 X-2.4983 Z1.4113 A46.8
> N7 X-2.5389 Z1.404 A46.3
> N8 Z1.4 A45.
> N9 X-2.5388 A43.7 F14.7
> N10 X-2.4959 A43.2
> N11 X-0.0018 A43.2
>
>
> Effectively the feed rate on the X,Y and Z is 11 IPM or 14.7 IPM. But
> the rotary axis is angular under LinuxCNC and measured in degrees per
> minute. I believe that makes sense because the diameter of the part
> being rotated determines the actual feed rate. So if the circumference
> was 14.7" and the cutting speed is set at 14.7 IPM then the rotary
> axis should turn 360 degrees per minute.
>
> But as shown in line N9 we have simultaneous motion on X and A but at
> F14.7.
>
> Clearly if the diameter was such that the circumference was 29.4" then
> the feed rate of the A axis would have to be half or 180
> degrees/minute.
>
> Running the G-Code above sees the Z or X axis moving at the expected
> speed.  Watching paint dry is more interesting than watching the A
> axis turn.  But if I just do a G1 A360 F360 the motion of the A axis
> at 4.68 diameter  appears to be about the same speed  as the X or Z
> horizontally.  It also takes exactly 1 minute to move 360 degrees at
> 360 degrees/minute.
>
> So how is this solved?   How would the A axis know the diameter and be
> able to translate that a request of F14.7 should really be F360 when Z
> is being moved at the same time?  Odds are I've configured the CAM
> software wrong but if I was going to just manually write some G-Code
> that involved simultaneous motion what would I do?
>
> The AXIS display shows 14.7 for speed.  The Z is known.  Is there
> something missing so that the A axis actually gets a much faster rate?
>
See, in LinuxCNC_Documentation.pdf, the G93-94-95 versions of how a feed 
rate in interpreted. You probably want G93, with a < 1.0 feed rate for 
starters. A F0.25 would take 4 minutes for the A move, with any other 
axises in that _same command line_ slaved to the A progress. F0.5 would 
take 2 minutes.   Note that is effective only for the line it begins, 
and reverts to normal motion then line is completed. 

I haven't used it enough to be a spurt. let alone an expert so fire up 
your favorite pdf viewer and read it starting at G93 to make sure. Any 
conversions of degrees to linear speed, similar to CSS, will have to be 
done in the gcode, I think...  I've carved drill bits for wood working 
that way by making the spiral with a round nosed bit. Didn't work like a 
$25 bit, but it did get the job done. I was planting short (16") 4x4's 
on the front deck, dropping/driving the 4x4 post to hold a plastic fence 
on one side of the wheelchair ramp I built when the missus fell & broke 
a hip. Came out a heck of a lot more rigid than I thought it was going 
to be.

> Thanks
> John
>
>
>
>
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users


Cheers, Gene Heskett
-- 
"There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order."
-Ed Howdershelt (Author)
If we desire respect for the law, we must first make the law respectable.
 - Louis D. Brandeis
Genes Web page 


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Rotary axis usage

2019-07-22 Thread John Dammeyer 
Hi Martin,
May be a fast short  reply but the first minute of the video completely 
described the problem.  While on doggy walk this morning pondering the problem 
I knew the solution had to be as described in the video.  But I didn't realize 
there is a G93 that is used in conjunction with a post processing of the G-Code 
file.  A very simple solution.

Didn't think I was running into something new.  But that video link you posted 
didn't show up when I googled the problem.  And most forum posts were also even 
ignorant of the issue which really surprised me.

Thanks
John


> -Original Message-
> From: Martin Dobbins [mailto:tu...@hotmail.com]
> Sent: July-22-19 12:22 PM
> To: Enhanced Machine Controller (EMC)
> Subject: Re: [Emc-users] Rotary axis usage
> 
> Real fast reply John, but does this video help?
> 
> https://www.youtube.com/watch?v=d0ffiCekhpE
> 
> Martin
> 
> 
> From: John Dammeyer 
> Sent: Monday, July 22, 2019 12:06 PM
> To: 'Enhanced Machine Controller (EMC)'  us...@lists.sourceforge.net>
> Subject: [Emc-users] Rotary axis usage
> 
> I've run into a situation with the CAM file generated by MECSOFT AlibreCAM
> appears to have a problem.  I've asked this on the support group for
> AlibreCAM but I think it's a more general question involving simultaneous 4
> axis milling where I write the G-Code myself.
> 
> 
> N1 G17 G20 G40 G90
> (4th Axis Create Cylinder/Round)
> N2 T2 M06
> N3 S2 M3
> N4 G0 X-2.2788 Y0. Z1.664 A46.8 F0.
> N5 G1 Z1.45 A46.8 F11.
> N6 X-2.4983 Z1.4113 A46.8
> N7 X-2.5389 Z1.404 A46.3
> N8 Z1.4 A45.
> N9 X-2.5388 A43.7 F14.7
> N10 X-2.4959 A43.2
> N11 X-0.0018 A43.2
> 
> 
> Effectively the feed rate on the X,Y and Z is 11 IPM or 14.7 IPM. But the
> rotary axis is angular under LinuxCNC and measured in degrees per minute.
> I believe that makes sense because the diameter of the part being rotated
> determines the actual feed rate. So if the circumference was 14.7" and the
> cutting speed is set at 14.7 IPM then the rotary axis should turn 360 degrees
> per minute.
> 
> But as shown in line N9 we have simultaneous motion on X and A but at
> F14.7.
> 
> Clearly if the diameter was such that the circumference was 29.4" then the
> feed rate of the A axis would have to be half or 180 degrees/minute.
> 
> Running the G-Code above sees the Z or X axis moving at the expected
> speed.  Watching paint dry is more interesting than watching the A axis turn.
> But if I just do a G1 A360 F360 the motion of the A axis at 4.68 diameter
> appears to be about the same speed  as the X or Z horizontally.  It also takes
> exactly 1 minute to move 360 degrees at 360 degrees/minute.
> 
> So how is this solved?   How would the A axis know the diameter and be
> able to translate that a request of F14.7 should really be F360 when Z is
> being moved at the same time?  Odds are I've configured the CAM software
> wrong but if I was going to just manually write some G-Code that involved
> simultaneous motion what would I do?
> 
> The AXIS display shows 14.7 for speed.  The Z is known.  Is there something
> missing so that the A axis actually gets a much faster rate?
> 
> Thanks
> John
> 
> 
> 
> 
> 
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users
> 
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Rotary axis usage

2019-07-22 Thread Martin Dobbins 
Real fast reply John, but does this video help?

https://www.youtube.com/watch?v=d0ffiCekhpE

Martin


From: John Dammeyer 
Sent: Monday, July 22, 2019 12:06 PM
To: 'Enhanced Machine Controller (EMC)' 
Subject: [Emc-users] Rotary axis usage

I've run into a situation with the CAM file generated by MECSOFT AlibreCAM 
appears to have a problem.  I've asked this on the support group for AlibreCAM 
but I think it's a more general question involving simultaneous 4 axis milling 
where I write the G-Code myself.


N1 G17 G20 G40 G90
(4th Axis Create Cylinder/Round)
N2 T2 M06
N3 S2 M3
N4 G0 X-2.2788 Y0. Z1.664 A46.8 F0.
N5 G1 Z1.45 A46.8 F11.
N6 X-2.4983 Z1.4113 A46.8
N7 X-2.5389 Z1.404 A46.3
N8 Z1.4 A45.
N9 X-2.5388 A43.7 F14.7
N10 X-2.4959 A43.2
N11 X-0.0018 A43.2


Effectively the feed rate on the X,Y and Z is 11 IPM or 14.7 IPM. But the 
rotary axis is angular under LinuxCNC and measured in degrees per minute.
I believe that makes sense because the diameter of the part being rotated 
determines the actual feed rate. So if the circumference was 14.7" and the 
cutting speed is set at 14.7 IPM then the rotary axis should turn 360 degrees 
per minute.

But as shown in line N9 we have simultaneous motion on X and A but at F14.7.

Clearly if the diameter was such that the circumference was 29.4" then the feed 
rate of the A axis would have to be half or 180 degrees/minute.

Running the G-Code above sees the Z or X axis moving at the expected speed.  
Watching paint dry is more interesting than watching the A axis turn.  But if I 
just do a G1 A360 F360 the motion of the A axis at 4.68 diameter  appears to be 
about the same speed  as the X or Z horizontally.  It also takes exactly 1 
minute to move 360 degrees at 360 degrees/minute.

So how is this solved?   How would the A axis know the diameter and be able to 
translate that a request of F14.7 should really be F360 when Z is being moved 
at the same time?  Odds are I've configured the CAM software wrong but if I was 
going to just manually write some G-Code that involved simultaneous motion what 
would I do?

The AXIS display shows 14.7 for speed.  The Z is known.  Is there something 
missing so that the A axis actually gets a much faster rate?

Thanks
John





___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

[Emc-users] Rotary axis usage

2019-07-22 Thread John Dammeyer 
I've run into a situation with the CAM file generated by MECSOFT AlibreCAM 
appears to have a problem.  I've asked this on the support group for AlibreCAM 
but I think it's a more general question involving simultaneous 4 axis milling 
where I write the G-Code myself.


N1 G17 G20 G40 G90
(4th Axis Create Cylinder/Round)
N2 T2 M06
N3 S2 M3
N4 G0 X-2.2788 Y0. Z1.664 A46.8 F0.
N5 G1 Z1.45 A46.8 F11.
N6 X-2.4983 Z1.4113 A46.8
N7 X-2.5389 Z1.404 A46.3
N8 Z1.4 A45.
N9 X-2.5388 A43.7 F14.7
N10 X-2.4959 A43.2
N11 X-0.0018 A43.2


Effectively the feed rate on the X,Y and Z is 11 IPM or 14.7 IPM. But the 
rotary axis is angular under LinuxCNC and measured in degrees per minute.
I believe that makes sense because the diameter of the part being rotated 
determines the actual feed rate. So if the circumference was 14.7" and the 
cutting speed is set at 14.7 IPM then the rotary axis should turn 360 degrees 
per minute.

But as shown in line N9 we have simultaneous motion on X and A but at F14.7.

Clearly if the diameter was such that the circumference was 29.4" then the feed 
rate of the A axis would have to be half or 180 degrees/minute.

Running the G-Code above sees the Z or X axis moving at the expected speed.  
Watching paint dry is more interesting than watching the A axis turn.  But if I 
just do a G1 A360 F360 the motion of the A axis at 4.68 diameter  appears to be 
about the same speed  as the X or Z horizontally.  It also takes exactly 1 
minute to move 360 degrees at 360 degrees/minute.

So how is this solved?   How would the A axis know the diameter and be able to 
translate that a request of F14.7 should really be F360 when Z is being moved 
at the same time?  Odds are I've configured the CAM software wrong but if I was 
going to just manually write some G-Code that involved simultaneous motion what 
would I do?

The AXIS display shows 14.7 for speed.  The Z is known.  Is there something 
missing so that the A axis actually gets a much faster rate?

Thanks
John





___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users