Setting up machine time in rotary turning

Topics related to wrapped rotary machining in Aspire or VCarve Pro
Post Reply
kcspeltz
Vectric Apprentice
Posts: 59
Joined: Tue Nov 02, 2010 6:05 pm
Model of CNC Machine: New CNC
Location: Minnesota City,MN

Setting up machine time in rotary turning

Post by kcspeltz »

Should there be different set up procedure for setting up machine times for doing the rotary turning.My time was showing to do the job in about 4 1/2 hours and it actually took about 9 1/5 hours any suggestion.

Kris

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: Setting up machine time in rotary turning

Post by Greolt »

Kris

If you are using Mach3 as your controller then I can help. :)

Greg

kcspeltz
Vectric Apprentice
Posts: 59
Joined: Tue Nov 02, 2010 6:05 pm
Model of CNC Machine: New CNC
Location: Minnesota City,MN

Re: Setting up machine time in rotary turning

Post by kcspeltz »

Yes, I am using Mach3

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: Setting up machine time in rotary turning

Post by Greolt »

OK, are you using "rotary axis feedrate compensation"?

Greg

kcspeltz
Vectric Apprentice
Posts: 59
Joined: Tue Nov 02, 2010 6:05 pm
Model of CNC Machine: New CNC
Location: Minnesota City,MN

Re: Setting up machine time in rotary turning

Post by kcspeltz »

I don't think so, is that on Aspire or on Mach3 ? Sorry for not being all acquainted with my software and programs as I just got into CNC last August.

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: Setting up machine time in rotary turning

Post by Greolt »

What I would guess is happening, is that the moves involving the 4th axis are much slower than what Aspire/Vcarve is calculating job time with.

The following is a copy of a post I made a while ago. It may help with understanding what is going on.

--------------------------------------------------------------------------------------------------

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

So what is 60 ipm on the linear axis (desired speed of the tool in the work), is 60 degrees per min for the rotary.

That 60 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 "Rotation Offset Radius"

They are to tell Mach the distance that the relevant axis origin (Z in this case) 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 Offset 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 Offset Radius" 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 Offset 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 Offset Radius" DRO will automatically disable the entire feedrate compensation feature.  This is a known bug 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 Offset Radius" DRO when zero is the correct and desired value.  Small enough to have no measurable effect on feedrate, but not zero.

Hope that all makes sense.  

Greg

kcspeltz
Vectric Apprentice
Posts: 59
Joined: Tue Nov 02, 2010 6:05 pm
Model of CNC Machine: New CNC
Location: Minnesota City,MN

Re: Setting up machine time in rotary turning

Post by kcspeltz »

Thanks ,I have something running on the CNC now so when it is done I'll take a look at those settings.

Kris.

kcspeltz
Vectric Apprentice
Posts: 59
Joined: Tue Nov 02, 2010 6:05 pm
Model of CNC Machine: New CNC
Location: Minnesota City,MN

Re: Setting up machine time in rotary turning

Post by kcspeltz »

In the toolpath page I don't see or can't find the toolpath set up menu. Is it on the main toolpath page or is it in one of the drop down menus ? Are there different versions of Mach3 ?

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: Setting up machine time in rotary turning

Post by Greolt »

It is in the drop down menu.

I am not in front of my computer right now, so can not give the exact menu position.

Greg

Post Reply