Wrapping With Mach

[dewalt58]

Thanks Greg, the hotkeys were the perfect solution!! I forgot completely about em!! Ok, now another question...did a wrap with Aspire's wrapper. I noticed that each time my tool path on the A-axis advanced from +000.0000 degrees to -360.0000 to make one pass and then needed to go back to +000.0000 degrees, it would reverse direction to do it instead of just going the same direction (1 degree) to get there. There by taking 4 mins to do this reverse rotation while program waits for it. Is this normal? Is there something I'm missing here in setting up Mach3?

AL

[Greolt]

First thing is, 4 mins to do one rotation is very slow.

Is it cutting as it goes back to zero or is it a rapid move?

Any way if your toolpath cuts back and forth before wrapping it will do the same when wrapped. So do a toolpath that cuts back and forth.

I usually make my toolpath so that it cuts back and forth in line with the axis. So the rotary axis only turns the amount of stepover each cut.

If using Mach there are things to have set so that the rotary axis feedrate is compensated to allow for different diameters.

Takes a bit of explaining and I am about to go out the door for a week away from computers.

All to do with "Rotation Radius" DROs and "Use Radius for Feedrate" and how they interact, to do the feedrate compensation.

Greg

[DavidCousins]

Hi Guys,
I just finished building my 4th axis. I've been away from home 3 weeks out of 4, so I can't work on the build. But this weekend I'm home and I've been building. I almost ready to cut some wraps.

I have a question. How do I calculate steps/inch, or steps/rev, or steps/degree? What is Mach3 using for units in the denominator. I'm pretty sure it's degrees, but I just want to make sure.
Thanks,
Dave

[kilrabit]

You are going to use 360 per revolution. Your screen will not say degrees, it will be units.

When using the motor tuning, when you put 360 it will be 1 revolution.

[dewalt58]

Greg....I got it figured out now! Its working fine!
Dave ...I made some notes over at Joe's forum about setting up Mach3, look in the Aspire Tutorial section.


AL

[DavidCousins]

Greg,
Did you get back from your travels yet? I'm getting the same slow moves that Al got. I've looked into Mach for setting to input a diameter, but I'm not seeing an input field. If you have time to weigh in on the subject, I'd appreciate it.

Al, You've sure helped me a bunch, thanks. I still think there's something missing about the cutting speeds of the Rotary that Mach should be computing.

Thanks guys,
Dave

First thing is, 4 mins to do one rotation is very slow.

Is it cutting as it goes back to zero or is it a rapid move?

Any way if your toolpath cuts back and forth before wrapping it will do the same when wrapped. So do a toolpath that cuts back and forth.

I usually make my toolpath so that it cuts back and forth in line with the axis. So the rotary axis only turns the amount of stepover each cut.

If using Mach there are things to have set so that the rotary axis feedrate is compensated to allow for different diameters.

Takes a bit of explaining and I am about to go out the door for a week away from computers.

All to do with "Rotation Radius" DROs and "Use Radius for Feedrate" and how they interact, to do the feedrate compensation.

Greg

[Fleming]

I am having the same problem as Dave (I think ). I have everything working but am confused about the speed of the rotary. I resolve this by putting in the diameter of the stock in Rotation Diameters (Settings Screen) within Mach3. Was wondering if the PP for Vectric could be modified to automatically put this value into Mach3???

[olf20]

Here is a link to one of Greg's posts that gives a wealth of information on 4th axis
machining, with Aspire, VcarvePro, and Mach3. Its long but filled with valuable
information.
olf20 / Bob

[Greolt]

Mach3 has a feature to compensate the rotary axis feedrate in an attempt to have the actual feedrate at the tool to be what is commanded in the gcode.

This feature has had a long standing bug which was only recently been 90% fixed. You must have at least Version 3.042.033

"Use Radius for Feedrate" must be ticked in Menu/Config/Toolpath. (It used to be labelled "Use Diameter for Feedrate")

And also there must be some value greater than zero in the "Rotation Radius" DRO (It used to be labelled "Rotation Diameters") which is found on the Settings page.

IMPORTANT NOTE: A Setting of Zero will turn this feature off. This little bug is the 10% we did not get fixed. Hopefully soon.

To do this feedrate compensation, Mach takes two DRO values into consideration. The Z axis DRO and the Rotation Radius DRO

I strongly recommend always using the centre of rotation as Z zero. There are lots of good reasons for Mach users to make this a habit.

In this case you need a very small value in the "Rotation Radius" DRO.

I suggest some thing like "0.01". Small enough to have no real effect but NOT ZERO.

IF YOU WANT TO use the surface of the material as Z zero, then you must place that radius value in the "Rotation Radius" DRO

Greg

[dewalt58]

Greg.......I'm running the latest version of Mach3 V3.042.036 and it still shows "Rotation Diameter" on the settings screen! Not "Roataion Radius" But Config, Toolpath does say "Use radius for feedback", could this be because I'm running the "BLUE SCREEN SET" and not the normal standard screen set?
Everything apears to be working ok while doing a wrapper run.

AL

[Greolt]

Yes that screenset is an old one somebody made up. Third party.

It is really a bit out of date. Mach has had a number of changes since then.

Greg

[dewalt58]

Thanks Greg, that confirms my suspision of the "Blue Sreen Set" , it just dawned on me tonight that it could be the problem of my misunderstanding when you kept saying, "Rotational Radius" on the "settings Screen"....But as long as its just a small thing, I'll keep using the "Blue", I like it!!


AL

[Greolt]

Have a look at this jpg. I could not match the font exactly.

If you want, then just put it in the "bitmaps/Mach Test Screens" folder and overwrite the old one.

Greg

[dewalt58]

Thanks Greg!!! Thats great!! It worked perfectly!! Got er done!!!


AL

[DavidCousins]

Greg.
Thanks for the info. I'll upgrade when I get home to Alabama. Now I have to wait 21 days. It will be the first thing that happens.
Thanks
Dave

Mach3 has a feature to compensate the rotary axis feedrate in an attempt to have the actual feedrate at the tool to be what is commanded in the gcode.

This feature has had a long standing bug which was only recently been 90% fixed. You must have at least Version 3.042.033

"Use Radius for Feedrate" must be ticked in Menu/Config/Toolpath. (It used to be labelled "Use Diameter for Feedrate")

And also there must be some value greater than zero in the "Rotation Radius" DRO (It used to be labelled "Rotation Diameters") which is found on the Settings page.

IMPORTANT NOTE: A Setting of Zero will turn this feature off. This little bug is the 10% we did not get fixed. Hopefully soon.

To do this feedrate compensation, Mach takes two DRO values into consideration. The Z axis DRO and the Rotation Radius DRO

I strongly recommend always using the centre of rotation as Z zero. There are lots of good reasons for Mach users to make this a habit.

In this case you need a very small value in the "Rotation Radius" DRO.

I suggest some thing like "0.01". Small enough to have no real effect but NOT ZERO.

IF YOU WANT TO use the surface of the material as Z zero, then you must place that radius value in the "Rotation Radius" DRO

Greg