Rotary seems to run slower than ..........

Topics related to wrapped rotary machining in Aspire or VCarve Pro
MikeUSNRet
Vectric Craftsman
Posts: 215
Joined: Wed Apr 21, 2010 3:51 pm

Rotary seems to run slower than ..........

Post by MikeUSNRet »

While away from work this week, I am attempting to finally get out and try some litho's in pvc pipe.

My rotary seems to be running terribly slow even with a feed-rate of 150 ipm. on flat stock, this would zip right through.

In Mach 3 under settings -> Motor Tuning for my A axis, I have 35.555555 set in as my Steps Per value.

Here is how I derived at this number:

Nema 23 460Oz/in stepper 1.8 steps per degree or 200 steps per rev (360 deg)
Driver set to 1/16 microstepping

Using a pulley system where I have an 18tooth gear on the stepper and a 72 tooth gear on the rotary giving a 4:1 ration

So If I take 200 * 16 * 4 that gives me 12800 and then I divide by 360 and I get 35.55555

Mathwise, this is correct, but somehow something seems amiss when the axis seems to be turning so slow.

ideas or suggestions for solution?

Kind of frustrating when Aspire says this job should take 28 minutes and it is well beyond that.
STGC(SW/AW) M. Wenman USN Ret.
1982 - 2005

Greolt
Vectric Wizard
Posts: 992
Joined: Fri Sep 21, 2007 1:44 pm
Model of CNC Machine: UCCNC Router, Plasma, Laser
Location: Australia 3781

Re: Rotary seems to run slower than ..........

Post by Greolt »

Mike

Your code calls for 150 units per minute.

So the rotary axis moves at a maximum of 150 degrees per minute. Snail pace.

Mach3 has a rotary axis feedrate compensation feature to address this.

I can write more on this when I get home, but in brief;

Under toolpath menu, select "Use Radius for Feedrate"

Set the distance that Z origin is offset from centre of rotation on the settings page.

Greg

MikeUSNRet
Vectric Craftsman
Posts: 215
Joined: Wed Apr 21, 2010 3:51 pm

Re: Rotary seems to run slower than ..........

Post by MikeUSNRet »

Re-checked and already had "A Rotations Enabled" checked and to use Radius for Feedrate. Under Settings, anything associated with Z was set to .0001 and yet it all still runs at a snails pace.

Grrrrr
STGC(SW/AW) M. Wenman USN Ret.
1982 - 2005

texark
Posts: 3
Joined: Tue Jul 10, 2012 12:59 am
Model of CNC Machine: Homemade

Re: Rotary seems to run slower than ..........

Post by texark »

A few things to check. Is the Yellow LED next to the A Axis DRO lit that says Radius Correct. If not it is not doing any radius compensation. Go to the Settings screen and under Rotation Radius top right of the screen and in the A Axis enter in 0.0001

On the General Config Page under Angular Properties there should be a check for A- Axis is Angular.

Everything else should be correct, did not check your math for the steps though. I have a 20.4:1 gear reduction and my steps are set to 22.666 but dont remember if I am doing microstepping in the controller.

To test your steps you should be able to put in in 360 on the Program Run page for Axis A and then press goto zero and the A-axis should rotate 1 revolution.

MikeUSNRet
Vectric Craftsman
Posts: 215
Joined: Wed Apr 21, 2010 3:51 pm

Re: Rotary seems to run slower than ..........

Post by MikeUSNRet »

Thanks Tex,

That was it. didn't have .0001 set in A-rotation in settings screen.
STGC(SW/AW) M. Wenman USN Ret.
1982 - 2005

Greolt
Vectric Wizard
Posts: 992
Joined: Fri Sep 21, 2007 1:44 pm
Model of CNC Machine: UCCNC Router, Plasma, Laser
Location: Australia 3781

Re: Rotary seems to run slower than ..........

Post by Greolt »

This is an explanation that I wrote a while ago.

===============================================================================

All axis move in units per min. With a rotary axis those units are degrees.

So what is 120 ipm on the linear axis (desired speed of the tool in the work), is 120 degrees per min for the rotary.

That 120 degrees per min angular feedrate will make the tool move through the work at a speed dependant on the distance the tool is away from the centre of rotation. (in your case, very slowly)

So Mach has a feature to compensate the rotary axis feedrate, to accommodate differing radius that the tool is cutting at.

It is activated via the Toolpath Setup menu. Check "Use Radius for Feedrate" All the other settings in this box are to do with the toolpath display window.

On the Settings page there are three DROs labelled "Rotation Radius". IMO they would be better labelled "Origin Offset from Centre of Rotation"

They are to tell Mach the distance that the relevant axis (Z in this case) origin, is offset from the centre of rotation. (A axis in this case)

So if you are machining on the outer surface of a 10 unit diameter job and Z axis origin (zero) is set on that outer surface, then the correct value for the "Rotation Radius" DRO is 5. The distance that Z origin is OFFSET from centre of rotation.

If, on the other hand, the Z axis origin is at the centre of rotation (my preferred method for most jobs) then the correct value for "Rotation Radius Offset" DRO is zero. The distance that Z origin is OFFSET from centre of rotation is zero.

Mach takes the Z axis DRO value and the "Rotation Radius" DRO value and adds them together to ascertain at what radius the tool is cutting at any one time. Then compensates the angular feedrate to have the tool move through the material at the desired speed.

Maximum velocity as set in motor tuning is honoured, so that will always be the upper feedrate limit.

Now there is one little "Gotcha". A zero value in the "Rotation Radius" DRO will automatically disable the entire feedrate compensation feature. This is a known bug in Mach3 and is being addressed by Artsoft at this time. Hopefully it will be fixed soon.

The workaround for this, is to use a very small value (eg. 0.001) in the "Rotation Radius" DRO when zero is the correct and desired value. Small enough to have no measurable effect on feedrate, but not zero.

====================================================================================

Regarding the two last paragraphs;

This bug in Mach 3 was fixed some versions ago. Not sure exactly when.

Another thing worth noting;

The "A- Axis is Angular" check-box does ONLY ONE thing. It stops the DRO for A axis being scaled when swapping from metric to imperial or vice versa. No other magic.

Greg

texark
Posts: 3
Joined: Tue Jul 10, 2012 12:59 am
Model of CNC Machine: Homemade

Re: Rotary seems to run slower than ..........

Post by texark »

Glad you got it working. Have some fun!

I've been playing-carving signs in white oak logs with the bark still on. Now if I can get the boring beatles killed that are still in the log I'll be happy.

Bill

MikeUSNRet
Vectric Craftsman
Posts: 215
Joined: Wed Apr 21, 2010 3:51 pm

Re: Rotary seems to run slower than ..........

Post by MikeUSNRet »

Now that I have the rotary axis zipping along just fine, running into another snag.

Orientation is X axis is bottom to top with +X at the top. and A rotates along Y Left to Right.

2 problems in this picture.

First, I had wanted to cut a border around the carving. I had the system set to cut at 120IPM.

The machine went to the bottom right corner, cut a nice straight line up to the top limits..began to rotate to cut along the top but before reaching the end, began arching down to the lower left corner. From there, another rotation with a nice straight line, but before reaching the end, as you can see, began another arc up to the right.

2nd problem:
As you can see in the picture, the top and bottom edges are nice and straight however we can see that the right edge does not go over all the way to the border and as it increases along the X axis, it begins a gradual curve inward. the left edge does curve outward as well, but not as drastic.

I had the file set to start in the lower left corner and cut at an angle of 315 deg.

Am sure that the rotary is missing steps, but this is pretty drastic. no indication that the belt on the reduction system is slipping and if it isn't, any ideas?
Attachments
rotary.jpg
STGC(SW/AW) M. Wenman USN Ret.
1982 - 2005

Greolt
Vectric Wizard
Posts: 992
Joined: Fri Sep 21, 2007 1:44 pm
Model of CNC Machine: UCCNC Router, Plasma, Laser
Location: Australia 3781

Re: Rotary seems to run slower than ..........

Post by Greolt »

Try it with CV turned off and see if that makes a difference.

Greg

MikeUSNRet
Vectric Craftsman
Posts: 215
Joined: Wed Apr 21, 2010 3:51 pm

Re: Rotary seems to run slower than ..........

Post by MikeUSNRet »

Doesn't matter if CV is on or off. Doesn't make any difference if cutting at a 45 deg angle, 0 deg or 90 deg so with that in mind, I started watching the rotary very closely. Seems as if the belt on the reduction setup has a little slop and at times also binds. back to the drawing board :(
STGC(SW/AW) M. Wenman USN Ret.
1982 - 2005

Jeff Johnson
Posts: 49
Joined: Mon Apr 12, 2010 2:53 am

Re: Rotary seems to run slower than ..........

Post by Jeff Johnson »

My rotary is turning extremely slow so I found this post, but it wont work on my setup. First of all I have a 4 axis table, my Y is 8 ft. , and my X is 4 ft. I am wanting to use my rotary up and down my Y axis. I am using my X as my rotary , or wrapping my X. So my A is always slaved to my Y. These setting will not work for my setup. Under Config, Gen Config , Angular Properties , there is no way to set X as angular. Is there a way to set the angular, or do I just give up and set it all up along my X. In the Mach tabs that is referenced here, there is no way to set X as angular drive its only A B or C ? Any help would be appreciated. Surely someone has a set up like this ?

Jeff Johnson
Posts: 49
Joined: Mon Apr 12, 2010 2:53 am

Re: Rotary seems to run slower than ..........

Post by Jeff Johnson »

Ok I found "my way" around this. Please tell me if its ok or not? i just assigned my X as B in mach, then I had to edit a post processor. I unplug my cables and run a different version of mach when I run normal anyway. So after running the rotary all I have to do is switch my A and X cables , open up the other program of mach and I am back to regular........Right?

Greolt
Vectric Wizard
Posts: 992
Joined: Fri Sep 21, 2007 1:44 pm
Model of CNC Machine: UCCNC Router, Plasma, Laser
Location: Australia 3781

Re: Rotary seems to run slower than ..........

Post by Greolt »

Jeff Johnson wrote: First of all I have a 4 axis table, my Y is 8 ft. , and my X is 4 ft. I am wanting to use my rotary up and down my Y axis.
So your rotary axis is parallel with the Y axis. Or to put it another way, it rotates about the Y axis. That is fine. You will "wrap" X positional values around the rotary. Quite normal.
I am using my X as my rotary , or wrapping my X.
You may be using the X axis driver (plugging the rotary into the X stepper driver) but you should still call the rotary "A"

There are good reasons for this, some of them are particular to how Mach works.

Set up a profile with the correct outputs assigned and start up Mach with that when doing rotary work.
So my A is always slaved to my Y.
Do you mean that the Y axis is dual drive and the A is slaved to Y?

If this is so then change the Y axis slave to be called "B" and keep the "A" definition free for the rotary.

Angular Properties , there is no way to set X as angular. Is there a way to set the angular,
Angular Properties are often misunderstood. This setting does just one thing and only one thing.
It tells Mach not to scale the output when changing from metric to imperial or vice versa.
No other magic in the background that many assume.
i just assigned my X as B in mach,
Don't do this. Assign the rotary "A" axis definition.

Mach can only visually represent an A axis toolpath. Not B or C.

Jeff Johnson
Posts: 49
Joined: Mon Apr 12, 2010 2:53 am

Re: Rotary seems to run slower than ..........

Post by Jeff Johnson »

Thanks Greolt , I was able to get it setup assigning the rotary as the "C" drive {never could get the "B" to act correct}. Had to re-edit a Post Processor , which was fun learning. Just getting into my hidden files on my computer was a challenge !!!! However my display doesn't do right so as I will take your suggestion when I get back to the shop. I will assign "B" or "C" as slave to "Y", then rotary as "A". Then my next hands on lesson will be designing a custom Mach screen. I have a 5 axis setup I got from CandCNC I would love to plug my rotary into the 5th drive plug and leave it but I never could quite put my head around what they were telling me from CandCNC so I just choose to plug and unplug "X" drive.Thanks for the help

Greolt
Vectric Wizard
Posts: 992
Joined: Fri Sep 21, 2007 1:44 pm
Model of CNC Machine: UCCNC Router, Plasma, Laser
Location: Australia 3781

Re: Rotary seems to run slower than ..........

Post by Greolt »

Jeff Johnson wrote: However my display doesn't do right so as I will take your suggestion when I get back to the shop. I will assign "B" or "C" as slave to "Y", then rotary as "A".
Yeah "A" is the way to go if you want a visuall toolpath representation.

Of course if you don't care about the toolpath view then "C" would be OK.
I have a 5 axis setup I got from CandCNC I would love to plug my rotary into the 5th drive plug and leave it but I never could quite put my head around what they were telling me from CandCNC so I just choose to plug and unplug "X" drive.
Stick with "plug and unplug "X" drive" until you get it all down pat, then move on to utilising the extra stepper driver if you feel the need.

Mach can handle up to six axis. On both my machines that have a rotary axis, I have "A" axis drivers. For true 4 axis work, or when I am using the 4th axis as an indexer.

Post Reply