How do you adjust feed rate on the rotary?

Topics related to wrapped rotary machining in Aspire or VCarve Pro
moto633
Vectric Wizard
Posts: 1123
Joined: Sun Jul 13, 2008 11:59 am
Location: Rockbridge, Ohio

How do you adjust feed rate on the rotary?

Post by moto633 »

Is there a way in Aspire to control the feed rate of the rotary axis "A" in my case. If i just set the feed rate for the tool to say 200ipm the rotary moves very slow. I know it is working in deg per min so how do I seperate that from general XY feed rates?

Thanks,
Nick

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: How do you adjust feed rate on the rotary?

Post by Greolt »

Aspire can not separate out A axis feedrates. The majority of moves will be blended anyway.

Two or more axis will move simultaneously to move the tool from one position to the next.

It is the job of the controller to blend the velocities of each axis during that move to have the tool move at the specified velocity.

The difficulty, as you have found, is that one axis is using a different base unit. Degrees rather than inches.

Controllers often have a way of compensating for this. Mach3 has a system to compensate the rotary axis feedrate.

ShopBot uses a feedrate scaling factor, which is addressed in the Post Processor.

What controller do you use?

Greg

moto633
Vectric Wizard
Posts: 1123
Joined: Sun Jul 13, 2008 11:59 am
Location: Rockbridge, Ohio

Re: How do you adjust feed rate on the rotary?

Post by moto633 »

Thanks Greg for your response.

I am running Wincnc on my new router. I think I am going to have to adjust some things in the INI file to get things going proper for my rotary.
I thought I was going to have time to mess with it today but time is running short!!

I will try again this week!!

Thanks,
Nick

cabnet636
Vectric Wizard
Posts: 2596
Joined: Fri Dec 21, 2007 1:57 am
Model of CNC Machine: CAMaster 508 ATC
Location: columbia sc
Contact:

Re: How do you adjust feed rate on the rotary?

Post by cabnet636 »

i tried to call you about this after we spoke today!
James McGrew
http://www.mcgrewwoodwork.com
CAMaster ATC 508 24/7 http://dropc.am/p/EJaKyl

moto633
Vectric Wizard
Posts: 1123
Joined: Sun Jul 13, 2008 11:59 am
Location: Rockbridge, Ohio

Re: How do you adjust feed rate on the rotary?

Post by moto633 »

phone was dead and we went to town to get new wireless stuff so I can get the camaster computer online in the shop for crosslink!! so far a total PITA!

I will get it so I can get help from you on line so we are on the same page!

cabnet636
Vectric Wizard
Posts: 2596
Joined: Fri Dec 21, 2007 1:57 am
Model of CNC Machine: CAMaster 508 ATC
Location: columbia sc
Contact:

Re: How do you adjust feed rate on the rotary?

Post by cabnet636 »

moto633 wrote:phone was dead and we went to town to get new wireless stuff so I can get the camaster computer online in the shop for crosslink!! so far a total PITA!

I will get it so I can get help from you on line so we are on the same page!

being online will speed the process up!!
James McGrew
http://www.mcgrewwoodwork.com
CAMaster ATC 508 24/7 http://dropc.am/p/EJaKyl

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: How do you adjust feed rate on the rotary?

Post by Greolt »

moto633 wrote:Thanks Greg for your response.

I am running Wincnc on my new router. I think I am going to have to adjust some things in the INI file to get things going proper for my rotary.
No worries Nick

I have no experience with WinCNC, so I will leave you in more capable hands. :)

Greg

820
Vectric Apprentice
Posts: 83
Joined: Wed Sep 30, 2009 12:57 am
Location: Goose Creek, SC

Re: How do you adjust feed rate on the rotary?

Post by 820 »

This is a little old but I have the exact same problem as moto633.
Greolt wrote:Aspire can not separate out A axis feedrates. The majority of moves will be blended anyway.
I'm using Cut2D and understand the blended moves.
Two or more axis will move simultaneously to move the tool from one position to the next.
Understood.
It is the job of the controller to blend the velocities of each axis during that move to have the tool move at the specified velocity.
Understood.
The difficulty, as you have found, is that one axis is using a different base unit. Degrees rather than inches.
Yes.
Controllers often have a way of compensating for this. Mach3 has a system to compensate the rotary axis feedrate.
I'm using Mach3 and would like to know the answer to fixing this problem.
ShopBot uses a feedrate scaling factor, which is addressed in the Post Processor.
No ShopBot here.
Any help would be much appreciated even a hint as to where I can find this in the Mach3 docs.

Thanks,
Ron (aka 820)

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: How do you adjust feed rate on the rotary?

Post by Greolt »

I know I have explained this before but can not find a thread to link to. So here goes,

Mach has a feature called "Use Radius for Feedrate".

To turn it on go to Menu/Config/Toolpath and check the box. Select the axis of rotation (strongly recommend using A) and check "A-Rotations Enabled"

Mach will calculate on the fly at what diameter the tool is cutting and compensate the rotary axis feedrate to allow for circumference changes.

The overriding limit being the max velocity as set in motor tuning of course.

To do this calculation Mach uses two values. The Z axis DRO and the "Rotation Radius" DRO found on the Settings page.

"Rotation Radius" DRO is the Z axis offset. If you have Z zero other than at centre of rotation, then this offset value goes in here.

For example if you want Z axis zero to be at the outer surface of a piece of round stock.

I always use the centre of rotation as Z axis zero and recommend this method.

So then the "Rotation Radius" DRO should read zero. Now here is where there is a GOTCHA.

Mach has a bug that turns off the "Use Radius for Feedrate" if there is a zero value in this DRO.

The workaround is the use a very small value, for instance I use "0.0001".

This has no effect on the compensation but prevents the feature being disabled.

Hope this helps,

Greg

820
Vectric Apprentice
Posts: 83
Joined: Wed Sep 30, 2009 12:57 am
Location: Goose Creek, SC

Re: How do you adjust feed rate on the rotary?

Post by 820 »

Greg,
Thanks for the quick reply...

I will give your advice a try in the morning. Using my rotary is like watching paint dry, I usually don't paint things just for that reason.

Thanks again,
Ron

820
Vectric Apprentice
Posts: 83
Joined: Wed Sep 30, 2009 12:57 am
Location: Goose Creek, SC

Re: How do you adjust feed rate on the rotary?

Post by 820 »

Greolt wrote:I know I have explained this before but can not find a thread to link to. So here goes,

Mach has a feature called "Use Radius for Feedrate".

I found "Use Diameter For Feedrate"
To turn it on go to Menu/Config/Toolpath and check the box. Select the axis of rotation (strongly recommend using A) and check "A-Rotations Enabled"
Toolpath is in the drop down from "Config"
Mach will calculate on the fly at what diameter the tool is cutting and compensate the rotary axis feedrate to allow for circumference changes.

The overriding limit being the max velocity as set in motor tuning of course.

To do this calculation Mach uses two values. The Z axis DRO and the "Rotation Radius" DRO found on the Settings page.

"Rotation Radius" DRO is the Z axis offset. If you have Z zero other than at centre of rotation, then this offset value goes in here.

For example if you want Z axis zero to be at the outer surface of a piece of round stock.
I use surface.
I always use the centre of rotation as Z axis zero and recommend this method.
I understand why but most of my rotary projects are simple engravings.
So then the "Rotation Radius" DRO should read zero. Now here is where there is a GOTCHA.

Mach has a bug that turns off the "Use Radius for Feedrate" if there is a zero value in this DRO.

The workaround is the use a very small value, for instance I use "0.0001".

This has no effect on the compensation but prevents the feature being disabled.
Entering the diameter of my stock seems to work.
Hope this helps,

Greg
Greg, this has helped me more than you'll ever know. I've been working with this for a while (like a year?) and hated to do any rotary stuff because it was so slow. Not now!!! Case in point, a 1" dia knob w/4 0.375" words took over an hour. DOC 0.030 in 2 passes.
After making the changes above cut time for the same file...3:29 minutes.
So now I can begin using and enjoying it so much more. Thank You!!!

Also, I need to give a shout out to Nick (MOTO633) for posting this question in the first place. I had done searches in the past on the other forums but always came up dry.

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: How do you adjust feed rate on the rotary?

Post by Greolt »

Ron

If your version says "Rotation Diameter" then you are using an older version of Mach.

The "Rotary Axis Feedrate Compensation" feature had some serious problems. The background calculations were being done wrong.

I worked with Brian Barker (Mach programmer) about 15 months ago, to get these sorted out.

This resulted in changes to this feature which came into being with Release 3.042.033. dated 23-12-09

The "Rotation Radius" name change happened then as part of that fix.

I suggest an upgrade to the latest version might be a good idea.

Greg

moto633
Vectric Wizard
Posts: 1123
Joined: Sun Jul 13, 2008 11:59 am
Location: Rockbridge, Ohio

Re: How do you adjust feed rate on the rotary?

Post by moto633 »

Very kind of you Ron! :D
I would think wincnc would have this ability to compensate like mach does..........it's only 10x the cost!!! :shock:
i do miss mach for a lot of things. Seems wincnc would be just as good or better with a lot of things. The one thing I miss is the detailed toolpath screen you can zoom in on in mach.

Glad Greg could help he is awesome!!

Best,
Nick

820
Vectric Apprentice
Posts: 83
Joined: Wed Sep 30, 2009 12:57 am
Location: Goose Creek, SC

Re: How do you adjust feed rate on the rotary?

Post by 820 »

Greg,
My mistake, I assumed that since you had posted the information from memory that what I found was correct.

I do have an older version of Mach3 (R3.041, Licensed on Jan 27, 2009). I have never given a thought to upgrading but will do it now.

Come to think about it now, I realise that I had been playing with the demo version that I downloaded right after Christmas 2009 and bought the license a month later.

Thanks for all your help and advise.

Ron

820
Vectric Apprentice
Posts: 83
Joined: Wed Sep 30, 2009 12:57 am
Location: Goose Creek, SC

Re: How do you adjust feed rate on the rotary?

Post by 820 »

moto633 wrote:Very kind of you Ron! :D
I was on the verge of removing my rotary since it was so slow, but this information has given it a whole new life. Thank you for asking the question.
I would think wincnc would have this ability to compensate like mach does..........it's only 10x the cost!!! :shock:
I'm just a hobbyist so I have to pinch my pennies.
I do miss mach for a lot of things. Seems wincnc would be just as good or better with a lot of things. The one thing I miss is the detailed toolpath screen you can zoom in on in mach.
I tried several programs before buying Mach3, I'm happy with that decision. Just wish that I could justify upgrading from Cut2D.
Glad Greg could help he is awesome!!
Agreed!!!

Thanks,
Ron

Post Reply