[PlanetCNC]

I don't get you. You can run any axis with any speed using G93.

[adidoro]

I don't get you. You can run any axis with any speed using G93.

I use CAD-CAM and generated g-code have 50000+ lines and a lot of G00 moves for positioning in 5 axis, so it's not practical to manually edit those lines. I don't have options in post processor to calculate those G00 moves with G93, it is only available on G01 and only when a rotary axis is involved.
Also it will be nice that g-code editor from Planet CNC software to have some functionality like notepad have, like go to line, search, find and replace and so on, else it's impossible to scroll trough editor to find where to edit. Or maybe when you double click on graphic area to jump in editor to that line like it does on the right panel.

[memphisjed]

I use CAD-CAM and generated g-code have 50000+ lines and a lot of G00 moves for positioning in 5 axis, so it's not practical to manually edit those lines. I don't have options in post processor to calculate those G00 moves with G93, it is only available on G01 and only when a rotary axis is involved.
Also it will be nice that g-code editor from Planet CNC software to have some functionality like notepad have, like go to line, search, find and replace and so on, else it's impossible to scroll trough editor to find where to edit. Or maybe when you double click on graphic area to jump in editor to that line like it does on the right panel.

I have tried to follow what is going on. To make it easier for those of us at home maybe define your a/b with degrees and not length. It makes everything easier. Your max spin speed is defined in the motor settings, no matter what your code calls for this will be max. There is also a max machine setting, again you will not go faster than this- the more axis the slower each one becomes- summations of each axis is max.
Interpolation is curves, not lines as in point to point you show. This is a 180 direction change so smoothing function will not be used. Point to point is brute force code and not as smooth as curves or supernubs. That aside it sounds more like a hardware issue: does each motor have its own power supply? If not at least a regen clamp on the dc side? As each axis stops there is a current backdrive to the power supply- if motors are all on the same the reversed current will find lowest resistance motor. This is usually a rotary with minimal weight.
5 axis simultaneously is a tall task for any controller, some are better than others. If you are expecting 1000 ipm on all five simultaneously you need a better (read expensive) controller- scales in all axis and resistor packs on each servo. If you are going 100 ipm the controller should handle it. Use Ethernet over usb, and turn your look ahead up a few clicks.
Turning up look ahead does slow the pause button which is something I wish could be fixed.

[adidoro]

Thank you for your reply.
The rotary axis B&C are in steps/degree is the only option in Planet CNC Controller settings. I agree with you with motor settings speed, that is the problem, because my linear axis are set to 2000mm/min max and when rotary axis is involved in that motion is restricted to speed of linear axis even it can go up to 8000 or more. That is why I stated and asked for Planet CNC how rotary axis speed is calculated, because being 3 time slower than linear axis I do my setting accordingly, but then that rotary axis will be restricted by that 2000mm/min on moving. I need to cite myself because no one seems to read that:

This question had also no answer.
I did the following test:
Moved machine in linear motion G43 G01 X100 F200 and I timed 30 seconds (obviously).
Than I zero machine to Y axis (rotary).
Than moved Z axis up at 15.922 witch is roughly the radius of a circle length of 100 mm and run the code G43 G01 B360 F200 witch was timed 108 seconds instead of 30 seconds for 100 mm at 200mm/min speed, so more than 3 time slower than linear motion.
Please test it, or if I did something wrong, tell me.

Now take a look at this video and see the engraving speed with G93 and the speed of G00 moves between cuts for positioning, and it's definitely not a hardware issue.

Or better here at 0:12 for example X axis change direction but trajectory only a bit and it stop

EDIT: first video related to rotary axis speed, second video related to interpolation move.

[memphisjed]

Thank you for your reply.
The rotary axis B&C are in steps/degree is the only option in Planet CNC Controller settings. I agree with you with motor settings speed, that is the problem, because my linear axis are set to 2000mm/min max and when rotary axis is involved in that motion is restricted to speed of linear axis even it can go up to 8000 or more. That is why I stated and asked for Planet CNC how rotary axis speed is calculated, because being 3 time slower than linear axis I do my setting accordingly, but then that rotary axis will be restricted by that 2000mm/min on moving. I need to cite myself because no one seems to read that:

Now take a look at this video and see the engraving speed with G93 and the speed of G00 moves between cuts for positioning, and it's definitely not a hardware issue.
https://www.youtube.com/watch?v=lcQELupZg3g
Or better here at 0:12 for example X axis change direction but trajectory only a bit and it stop https://youtu.be/7SzodArv3YU?t=12

B 360 f200 should take 108 seconds. Speed gets all sorts of weird to guess with rotaries. Your cam software has to do that math. F is speed in units/minute. A degree is a unit treated the same as mm or inch. It looks like your cam is not adjusting speed (f) as the rotation stops and motion is just xy. 5 axis cam takes a lot of tweaks to get right, and even then usually takes hand edits of code to get right. You can test controllers ability by slowing feed down until smooth and jacking speed up to see when it stutters or skips lines.

You can allow helical moves in the cam post- this should remove a lot of lines of code and put more math into the controller which should help smooth some of your motion out. Adjust smoothing function in controller up a tiny bit, adjust cam smoothing up a fair amount, add a few more counts on look ahead (though with Ethernet it does not need many). Cam has tolerance of machine variables, turn those way down for knunion work. If doing 5 axis work then you really need a 5 axis cam.

I see code errors, not control errors- which are usually truncated lines or square or starburst circles- extreme miss alignment of axis on rotation and other oddities.

[adidoro]

B 360 f200 should take 108 seconds

WHY?

There is no XY motion where it stops, is only C (or A for some, anyway rotary axis) X and Z movements. When X change direction but only a small trajectory change it stop, is not normal, exactly at the 180 degree of rotary move from 360.
The CAM that generate G-code is Camworks, I don't think is a CAM problem either.
I had the same problem in vectric aspire in 4 axis, in regard to rotary speed.

It looks like your cam is not adjusting speed (f) as the rotation stops and motion is just xy

Contrary it adjust (slower the rotary) when a linear axis moves, when not is fast, does not stop there.

FOR NOT CONFUSING THINGS
first video is about rotary speed that is one problem.
the second video is related to blend motion in 5 axis, witch was answered by Planet CNC

Because it is possible to calculate "blend" between two linear axes to smooth transition.
But B axis does not represent linear motion and blending is not possible. Good CAM will solve this because motion will be optimized.

That's not true, but anyway let's stick to rotary being slower than it should, regardless of 5 axis, take just 4 in consideration is the same thing.

[memphisjed]

WHY?
There is no XY motion where it stops, is only C (or A for some, anyway rotary axis) X and Z movements. When X change direction but only a small trajectory change it stop, is not normal, exactly at the 180 degree of rotary move from 360.
The CAM that generate G-code is Camworks, I don't think is a CAM problem either.
I had the same problem in vectric aspire in 4 axis, in regard to rotary speed.

Running iso to curve might force cam works to update feed rates. Almost every line in 5 axis contouring has a f command. Might need to play with post to get what you are after. Controllers are units per time on feed. B360 f 200 is 200 degrees per minute, 108 seconds for 360 degrees. X255 y255 f200 is about 108 seconds. Distance is sqrt(x^2+y^2+a^2+b^2+z^2). The mill has no idea of the speed relative to the surface. It only knows movement, not the underlying geometry.
Camworks has hours of training, minor post editing, and settings suggestions for your machine as part of maintance cost. Take advantage of that- you all ready pay for it. It has known jittering issues with a few bells turned on and whistles off it seems to work- which bells and whistles is on them.

[adidoro]

Every time you want a solution for a problem is to simplify to it's lower form it can be simplified.
So, if I type G00 B180 for example it will go fast to that position showing something like 8000+ on speed, if I type G00 B180 X1 will go much slower even if X it's moving only 1mm it will not reach that axis speed limit, instead will lower the rotary speed to linear axis maxim speed, so the linear axis will move only at maybe 200mm/min. Got it?
Don't complicate it to 5 axis, or smoothing tool path, it's not about that. It's only 2 AXIS one linear and one rotary.
About Camworks, I know more then that. I do not own a license I can't afford that, I only have access to a computer with solidworks and camworks for some services that I made for that company, those not matters here.

[PlanetCNC]

You are incorrect. Here are examples with calculations:

;example 1
;X - max speed = 10 mm/min
;C - max speed = 3600 deg/min
;Move from X0 C0 to X2 C180
;timeX = 2 / 10 * 60 = 12s ;this is slowest axis
;timeC = 180 / 3600 * 60 = 3s
G21 G90 G94
G00 X0 C0
(sw_reset)
;this move will take 12s as calculated
G00 X2 C180
(sw_print)




;example 2
;X - max speed = 1000 mm/min
;C - max speed = 360 deg/min
;Move from X0 C0 to X2 C180
;timeX = 2 / 1000 * 60 = 0.12s
;timeC = 180 / 360 * 60 = 30s ;this is slowest axis
G21 G90 G94
G00 X0 C0
(sw_reset)
;this move will take 30s as calculated
G00 X2 C180
(sw_print)




;example 3
;X - max speed = 10 mm/min
;C - max speed = 3600 deg/min
;Move from X0 C0 to X2 C180
;timeX = 2 / 10 * 60 = 12s ;this is slowest axis
;timeC = 180 / 3600 * 60 = 3s
G21 G90 G94
G00 X0 C0
(sw_reset)
G93
;this move will take 12s as set and as calculated
G01 X2 C180 F[60/12]
G94
(sw_print)




;example 4
;X - max speed = 10 mm/min
;C - max speed = 3600 deg/min
;Move from X0 C0 to X2 C180
;timeX = 2 / 10 * 60 = 12s ;this is slowest axis
;timeC = 180 / 3600 * 60 = 3s
G21 G90 G94
G00 X0 C0
(sw_reset)
G93
;this move will take 12s as calculated, 6s is set but not possible
G01 X2 C180 F[60/6]
G94
(sw_print)

[adidoro]

Look here and time it.
https://www.youtube.com/watch?v=g39EBcNZvTw

[adidoro]

Look here and time it.
https://www.youtube.com/watch?v=g39EBcNZvTw

1. From 0:02 to 0:04 C axis will move 360 deg. alone in 2 seconds.
2. From 0:08 to 0:23 X axis move 1mm together with C axis 360 deg. in 15 seconds.
3. From 0:25 to 0:29 X axis move back to zero 1mm and C axis back to 0 360 deg. but one by one, not together in 3 seconds.
(Timing was rounded to seconds for the sake of the video)

The POINT IS if you move 2 axis one by one in 3 seconds, combined movement should be less NO MORE!
You messed up calculations in the controller by applying the number of an linear axis move witch is in mm/min to a rotary axis witch is in deg/min. You can't do that, they are two different units of measures.

[PlanetCNC]

I did. Here are results. Exactly like I said.


The point is, that what you are saying is not true and my video shows it.
Please export your profile and send .zip file to our support mail. I'll check what is wrong with it.

[adidoro]

I did. Here are results. Exactly like I said.


The point is, that what you are saying is not true and my video shows it.
Please export your profile and send .zip file to our support mail. I'll check what is wrong with it.

Maybe if your traverse speed for X (linear axis) match your traverse speed for C (rotary axis). Mine not match. Because one is in mm/min and other in deg/min, different things exactly as I said!
Anyway I've sent my profile and waiting for answer.

[PlanetCNC]

This issue was resolved. Adidoro speed was limited because his "Program Option/Traverse Speed" was set wrong:

Program Option/Traverse Speed:

With this parameter you can set default speed value of traverse machine moves when G00 command is executed in program.

Motor/Speed:
You can set maximum speed of each axis motor. Motors will not exceed speed values set with these parameters.

[adidoro]

This issue was resolved. Adidoro speed was limited because his "Program Option/Traverse Speed" was set wrong:

Program Option/Traverse Speed:

With this parameter you can set default speed value of traverse machine moves when G00 command is executed in program.

Motor/Speed:
You can set maximum speed of each axis motor. Motors will not exceed speed values set with these parameters.

Indeed, thank you.
Somehow for me was counterintuitive because there are 2 settings in traverse speed, one for linear axis in mm/min and one for rotary axis in deg/min, so I was set 1500mm/min for linear and 8000deg/min for rotary.
But that setting of 1500mm/min for linear was constrained the rotary moves to that speed. I think it should not, but anyway problem fixed after setting that equal for both to 8000.

I have also a question, in the same Program Option there is a setting for Feed Speed in mm/min, that will apply the same for all axis even rotary witch are in deg/min?

[PlanetCNC]

In G94 mode, speed is defined as feed/minute.


If we have:
F100
G01 X100
Machine will travel one minute.


If we have:
F100
G01 C100
Machine will also travel one minute.


If we have:
F100
G01 X100 C100
This one is trickier. Total length used by TNG is 100 and not 141 because TNG assumes that those axes are from different system and that 141 makes no sense.
Machine will travel one minute.


F100
G01 X100 Y100
Now total length is 141. Machine will travel 85s


Special case is
F100
G01 X100 C200
Normally travel time is 2 minutes.
But C axis can be excluded from length calculation with Motion/Motion ABC setting.
If this is the case then travel time is 1 minute. C axis rotates at speed 200/min


In all cases above speed is set with F100.
If these is no F in g-code then last used speed will be used.
When you start TNG speed is set to value in setting Program Options/Feed Speed.


G00 move is similar. Only difference is, that it does not use F for speed.
Instead it uses speed from setting Program Options/Traverse Speed.
If only axes A, B or C are used then speed is from setting Program Options/Traverse Speed.


Regardless of speed set, Motor/Speed limits will never be exceeded.


Normally feed speed is also cut speed. But when rotary axes are involved this is not the case.
To calculate cut speed length of each move needs to be known. Because this depends on your machine construction TNG does not know this.
But your CAM does. And best way to do this is to use G93 (inverse time) mode.


G93
G01 X100 C100 F2
This move will take 30s regardless of anything else (apart from motor limits).
Because CAM calculates cut speed it known all times needed to perform moves and can set all F values correctly.


In other words - when any non linear axes are involved use G93.


Note that G00 traverse moves do not cut and cut speed does not apply. Therefore they always behave like G94 moves.
G00 should always move with fastest possible speed.

[adidoro]

Ok, I think I got it.
In other words that specific setting Program Option - Feed Speed does nothing except when you start the program and not specify a G01 F word it will use that setting.
In regard to G93, I already use it, and the cam calculate that when rotary axis is involved in cut moves.