Machsupport Forum

Mach Discussion => Mach4 General Discussion => Topic started by: lab auto man on January 21, 2019, 08:00:46 PM

Title: Finial switching over to Mach4 amd Ihave a few question.
Post by: lab auto man on January 21, 2019, 08:00:46 PM
Hi,
I gave up waiting for a Mach 4 USBSS plugin and bought a ESS to switch over to Mach 4.  I first got Mach 3 running with the ESS with little trouble but I did notice that homing my X axis sounded a little different.  My X axis has a slave motor and I could not tell if they were both homing.  I did not know it this was a difference between the USBSS and ESS or if only one motor was homing.  I went a head and got Mach 4 up and running with the ESS and my X axis homing is the same.  In Mach 3 their was a check box in the configuration page where you could check to say if you want both motors homed.  It squares up the gantry.  Is there something I am missing in Mach 4 to tell it to do the same thing?

My second question has to do with the rotary tool path display. So far it is much better the Mach 3 but is there way to adjust the diameter of what is displayed?   I did very little rotor stuff on my cnc router in Mach 3 but want to do more with mach 4.  The tool path look correct but the proportion is not correct.  In CAM it is long and thin but when I load the G code it is short and fat?  I think it may run ok if I ran it. 
Thanks for any help,
regards,
Todd
Title: Re: Finial switching over to Mach4 amd Ihave a few question.
Post by: joeaverage on January 26, 2019, 08:59:58 PM
Hi,
I don't have slaved axes so I can't answer definitively.

Slave motors are assigned to each axis on Configure/Control/Axis Mapping.

Each assigned slave motor will require its own Step and Direction pins and if you want to square the gantry each slave
will require its own home switch to complement the master home switch.

The gantry squaring routine is carried out by the ESS not Mach. Further details on how it works are probably best found
on the Warp9 site.

Craig
Title: Re: Finial switching over to Mach4 amd Ihave a few question.
Post by: joeaverage on January 26, 2019, 09:11:14 PM
Hi,

https://warp9td.com/index.php/kunena/7-general-discussion/7748-gantry-squaring-slave-sensor-not-registering#19732 (https://warp9td.com/index.php/kunena/7-general-discussion/7748-gantry-squaring-slave-sensor-not-registering#19732)

Craig
Title: Re: Finial switching over to Mach4 amd Ihave a few question.
Post by: lab auto man on January 29, 2019, 05:42:51 PM
Thanks Craig,

Now I have a rotary axis question for mach 4. I created some G code  in V carve to test the rotary axis.  My feed rate for my tool was 60 inch/min in v carve.  Mach 4 thinks it is 60 degree/min, to slow.

In mach 3 there was setting where you could tell mach it was a rotary job and it would compensate or adjust the speed.  Can I set that up in Mach 4?   Did I miss something in my setup?
I could make rotary tool in V carve software and crank the speed way up.
Thanks,
Todd
Title: Re: Finial switching over to Mach4 amd Ihave a few question.
Post by: joeaverage on January 30, 2019, 12:45:02 AM
Hi,
I don't use a fourth axis as so can't answer your question definitely.

I have heard that many have had success with using inverse time mode, this is a modal Gcode setting,
not a Mach4 setting.

Look up G93 page 54 in "Mill GCode Programming" manual in the Mcah4 Docs folder.

Craig
Title: Re: Finial switching over to Mach4 and Ihave a few question.
Post by: harlindg on March 25, 2019, 08:43:57 PM
Thanks Craig,

Now I have a rotary axis question for mach 4. I created some G code  in V carve to test the rotary axis.  My feed rate for my tool was 60 inch/min in v carve.  Mach 4 thinks it is 60 degree/min, to slow.

In mach 3 there was setting where you could tell mach it was a rotary job and it would compensate or adjust the speed.  Can I set that up in Mach 4?   Did I miss something in my setup?
I could make rotary tool in V carve software and crank the speed way up.
Thanks,
Todd



I have the same problem! If i set my CNC up as all METRIC when I use an INCH G-code file everything works great for rotary engraving feed speeds. If I set up my CNC for INCH & re-tune motors rotary speed is too slow! MACH4 with ESS Smoothstepper using VCarve files. Something is wrong in the MACH4 calculations for INCH to degrees! I've not got any answers on this problem that works - I would like to keep my Inch machine setup for 4th axis!
Title: Re: Finial switching over to Mach4 amd Ihave a few question.
Post by: joeaverage on March 25, 2019, 09:03:00 PM
Hi,
would you post the current axis max speeds and step per unit (all axes)?

What seems to happen when you have a rotary axis is that the linear axes go slow to stay in sync with the rotary axis,
especially if you have significant gear reduction in the rotary axis.

Craig
Title: Re: Finial switching over to Mach4 amd Ihave a few question.
Post by: harlindg on March 25, 2019, 10:22:34 PM
ESS CNC Rotary
The opposite happens - the linear axis (Y) 7 (Z) are OK its the wrapping of (X) which slows down. With th machine setup in MM all file works OK for both MM & Inch files. If I set the machine up for INCHES the inch files no longer feeds fast enough in the rotary axis. When I change motor 4 tuning I lose 360º per rev.
Title: Re: Finial switching over to Mach4 amd Ihave a few question.
Post by: joeaverage on March 25, 2019, 11:19:15 PM
Hi,

Quote
When I change motor 4 tuning I lose 360º per rev.

You can't change the tuning of your rotary axis WITHOUT changing the gearing or microstepping. With given
gearing and mircostepping there is a certain number of pulses required to rotate the axis one degree....set it
and leave alone.

You are moving axes in a coordinated fashion, the slowest axis determines the rate at which the other axes move.

Please post your axis tunings (steps per and max vel.)

Craig
Title: Re: Finial switching over to Mach4 amd Ihave a few question.
Post by: harlindg on March 26, 2019, 09:09:34 AM
Here is the settings that work with CNC set for MM. If I setup for INCH & change X, Y, & Z and leave A alone the A axis now turns too slow when I use the same Gcode files.
Title: Re: Finial switching over to Mach4 amd Ihave a few question.
Post by: joeaverage on March 26, 2019, 02:25:09 PM
Hi,

You have these tunings:
X axis 160 steps per and 3200 mm/min
Y axis 160 steps per and 3200 mm/min
Z axis 320 steps per and 1600 mm/min
A axis 160 per degree and 3200 degree/min

Note the A axis seems pretty slow, 3200 degrees per minute, or 8.888 revs/min or only 53.33 degrees/sec

Thus if you had a move in X and Y of 200 mm each combined with a rotation of 10 turns:

G0 X200 Y200 A3600

If we ignore the acceleration phase the move would take 3600/3200= 1.125 min to run. The linear axes appear to run slow
but it is because they have to slow down to stay in sync with the A axis.

It gets worse if you do a G1 move:

G1 X200 Y200 A3600 F300

Now, again ignoring the acceleration phase, would take 3600/300=12 minutes to run! This is because the machine
moves at the rate determined by the slowest axis, in this case A axis. The linear axes appear to move only 16.66mm/min.

This effect is exacerbated when you use inch units but it all stems from the fact that the rotary axis is slow and therefore
the linear axes must go very slow to stay in coordination with it.

Craig
Title: Re: Finial switching over to Mach4 amd Ihave a few question.
Post by: harlindg on March 26, 2019, 06:55:36 PM
Not sure I understand!  My X axis is motor 0, my Y axis is motor 1 & motor 3 (slave) and my A axis is the rotary axis - motor 4. When using the rotary CNC setup the Vcarve file sends the "Y" axis code to the "A" axis, as the "Y" axis stays at 0.000. My setting for the "A" axis is 26.7 counts per degree @ velocity of 4994 which rotates 1 rev for 360º. ( A axis is a belt driven 1:6 ratio)
Title: Re: Finial switching over to Mach4 amd Ihave a few question.
Post by: joeaverage on March 26, 2019, 07:48:21 PM
Hi,
OK I misinterpreted the motor tuning pages. Please disregard my previous post.

Motor0 X axis =160 at 3200 mm/min
Motor1 and Motor3 Y axis (and  slave)=160 at 3200 mm/min
Motor4 Z =26.7 at 4994 degrees/min

I assume you must use 8 microstep/full step to arrive at the figure 26.7 steps/degree?

Lets work on the same move I posted earlier:
G0 X200 Y200 A3600
If X (or Y) were the speed limiting axis then the move (excluding acceleration phases) would be 200/3200=0.0625
minutes or 3.75 sec. If the A axis is the speed limiting axis then the move would be 3600/4994=0.7208 minutes or 43.25 seconds.
Clearly the rotary axis is  the speed limiting axis, the linear axes slow down from their theoretical max to match the A axis.

Lets try the same machining move as before:
G1 X200 Y200 A3600 F300
Now the limiting axis is still the A axis rotating at 300 degrees per minute so the 10 revolutions of the A axis will take
12 minutes. The F word (300) applies a  maximum to ALL axes involved in the coordinated move, it this case the A axis
is moving therefore it is limited to 300 units/min or 300 degrees /min and the ten revolutions would require 12min to execute.

If the move were:
G1 X200 Y200 F300
Then the linear axes would be limited to 300mm/min and the move would execute in 200/300 =0.6666 min or 40secs

Lets now convert to inches per minute to see if anything changes.

Motor0 X axis =160x25.5=4064 steps per inch at 3200/25.4=126 inch/min
Motor1 and Motor3 Y axis= 4064 steps per at inch 126 inch/min
Motor4 A axis =26.7 steps per degree at 4994 degrees/min

G0 X8 Y8 A3600
Time to complete = 3600/4994=0.72 min or 43.25 sec, ie the same time. The linear axes have slowed from their theoretical best
of 126 inch/min to 8 inches in 43.25 seconds to maintain synchronization with the rotary axis.

Thus given that the rotary axis is slow it will determine the rate the linear axes travel.....not the linear axis maximums at all.

Craig