MechMate CNC Router Forum

Go Back   MechMate CNC Router Forum > After Building the Beast - Operating , Troubleshooting and Maintenance > Troubleshooting
Register Options Profile Last 1 | 3 | 7 Days Search Today's Posts Mark Forums Read

Reply
 
Thread Tools
  #1  
Old Wed 18 March 2009, 00:29
Kobus_Joubert
Just call me: Kobus #6
 
Riversdale Western Cape
South Africa
Send a message via Yahoo to Kobus_Joubert Send a message via Skype™ to Kobus_Joubert
Moves at different speeds for different directions - feed rates incorrectly defined

I was making some TRIM pieces last night when I noticed something odd. I was cutting 3mm deep slots with a 12mm ballnose. As each piece was only 1200mm long I set up to cut 1mm deep per pass. I pushed up the speed as there is not much friction. Old BBB took off cut at a nice fast pace, then suddenly slowed down on the next pass. When it starts the second slot it goes quickly and then when it cuts the second pass it slows down. On the Mach screen I saw the steps/distance decrease as well. Is this a Mach3 function or are my Gecko's 202's slowing down when it starts to pull amps under load, or is it maybe Cut2D that automatically generate G-Code as it goes deeper.

I never noticed it before when cutting odd objects (shapes)...or I did not notice it. When cutting something straight and simple it is very noticable.
Reply With Quote
  #2  
Old Wed 18 March 2009, 00:53
MariusL
Just call me: Marius #22
 
Centurion
South Africa
Kobus, you may have set the speed for the finishing pass slower than that of the first pass. If you increase the feed rate on Mach it does so by percentage. IE all feed rates will increase by that percentage.
Reply With Quote
  #3  
Old Wed 18 March 2009, 01:41
Gerald D
Just call me: Gerald (retired)
 
Cape Town
South Africa
Open your G-code with a text editor (eg. Wordpad) and look in there if you have a lot of F commands changing the feedrate. From the sounds of it, there must be. And they can only come from your g-code generator (Cut2D)

Your G202's cannot slow down under higher current draw.
Reply With Quote
  #4  
Old Wed 18 March 2009, 02:24
Kobus_Joubert
Just call me: Kobus #6
 
Riversdale Western Cape
South Africa
Send a message via Yahoo to Kobus_Joubert Send a message via Skype™ to Kobus_Joubert
Thanks for the feedback you two. Marius, in my Cut2D there is no difference in the setup that I can see. As Gerald suggested it must come from my Cut2D and the only logical explanation can be that the program decided that it must automatically include a feed change on certain passes. I will look at it again this afternoon.
Reply With Quote
  #5  
Old Thu 19 March 2009, 12:49
Kobus_Joubert
Just call me: Kobus #6
 
Riversdale Western Cape
South Africa
Send a message via Yahoo to Kobus_Joubert Send a message via Skype™ to Kobus_Joubert
I tried to cut another 2 pieces of TRIM....all it is, is 3 slots, 3,5,and 7mm deep and about 700mm long.

trim.jpg

I again noticed that the speed changes during certain cuts.
Here is the G-code as generated by cut2D and imported to Mach3

Profile 5.txt

Any suggestions ?
Reply With Quote
  #6  
Old Thu 19 March 2009, 14:22
Gerald D
Just call me: Gerald (retired)
 
Cape Town
South Africa
excerpt from g-code, spaces and colour added for clarity:
. . . . . .
. . . . . .
N80 X0.000 Y0.000 F240000.0
N90 G00 X5.905 Y56.931 Z6.000
N100 G01 Z-1.500 F6000.0
N110 G01 X705.905 F240000.0
N120 Y57.931
N130 X5.905
N140 Y56.931
N150 G01 Z-3.000 F6000.0
N160 G01 X705.905 F240000.0
N170 Y57.931
N180 X5.905
N190 Y56.931
N200 G00 Z6.000
N210 G00 Y140.008
N220 G01 Z-1.500 F6000.0

. . . . . .
. . . . . .

Looks like your Cut2D puts a z move feedrate F6000.0 after the z move, which is then used by the subsequent x and y moves?

(I think that Mach executes the codes in the sequence in which they appear on a line)
Reply With Quote
  #7  
Old Thu 19 March 2009, 23:47
Gerald D
Just call me: Gerald (retired)
 
Cape Town
South Africa
Correction to last post:

"Looks like your Cut2D puts a z move feedrate F6000.0 after the z move, which is then used by the subsequent x and y moves?"

The x-move going to the right (increasing x) is after a F6000, which is going to move the router at 6000mm/min.

But the x-move to the left (decreasing x) is after a F240000, which is going to try and move the router at 240 meters/min, but your motor's max speed setting will over-ride that down to your setting.
Reply With Quote
  #8  
Old Fri 20 March 2009, 00:11
Kobus_Joubert
Just call me: Kobus #6
 
Riversdale Western Cape
South Africa
Send a message via Yahoo to Kobus_Joubert Send a message via Skype™ to Kobus_Joubert
Thanks Gerald, I will play with the Z-Axis PLUNGE RATE in CUT2D and see if that changes anything.
Reply With Quote
  #9  
Old Fri 20 March 2009, 01:11
Gerald D
Just call me: Gerald (retired)
 
Cape Town
South Africa
Suggest you get onto the Vectric forum and check with them there. I wonder about having the feedrate appear after the move instruction in the same line?
Reply With Quote
  #10  
Old Fri 20 March 2009, 01:26
Kobus_Joubert
Just call me: Kobus #6
 
Riversdale Western Cape
South Africa
Send a message via Yahoo to Kobus_Joubert Send a message via Skype™ to Kobus_Joubert
My idea as well...just posted the same question there. Thanks
Reply With Quote
  #11  
Old Fri 20 March 2009, 06:33
J.R. Hatcher
Just call me: J.R. #4
 
Wilmington, North Carolina
United States of America
Send a message via Skype™ to J.R. Hatcher
As I understand, it doesn't matter where the F code is in the line. It does make a difference how X, Y, & Z codes are entered, they are executed in order ......... I think ........... I will check this out today.
Reply With Quote
  #12  
Old Fri 20 March 2009, 06:38
Kobus_Joubert
Just call me: Kobus #6
 
Riversdale Western Cape
South Africa
Send a message via Yahoo to Kobus_Joubert Send a message via Skype™ to Kobus_Joubert
Thanks JR, I had feedback on the Vectric forum and Brian said that the code is OK. So I take it that it does not matter where the F is in the line..something else is causing it to make it own decision on feed rate. Will do some AIR cuts this afternoon and note when it slows down and when it runs at normal speed...I am sure it was random....but will check.
Reply With Quote
  #13  
Old Fri 20 March 2009, 06:44
Richards
Just call me: Mike
 
South Jordan, UT
United States of America
Actually, the F6000.0 is for the Z move and F240000.0 is for the X and Y axis moves.

The line: N900 G01 Z-1.750 F6000.0 contains the following parameters:

N900 is the line number
G01 is the normal move command
Z-1.750 commands the Z-axis to move to the -1.750mm position
F6000.0 is the speed at which the Z-axis moves.


The line: N910 G01 X705.960 F240000.0 contains the following parameters:

N910 is the line number.
G01 is the move command
X705.960 commands the X-axis to move to the 705.960mm point
F240000.0 is the speed.

In both cases, the F-command could have been written before the axis command. The F-command is a persistent command that is associated with the line on which it first appears and then stays in effect for all subsequent G01 commands until you use another F-command.

It looks like the speed setting is wrong. 240,000mm per minute is 9,448-inches per minute or 157.48 inches per second! My guess is that the feed-rate for the tool that you're using was set wrong in the program that generated the G-code.

Edited: J.R. posted while I was writing. He and I agree that the axis and speed parameters are not position dependent in the parameter list.

I just ran this code on my test bench and it worked properly:

G01 F1000
X10
Y100
X0
Y0
X50
G00 X0

Last edited by Richards; Fri 20 March 2009 at 06:59..
Reply With Quote
  #14  
Old Fri 20 March 2009, 06:53
Kobus_Joubert
Just call me: Kobus #6
 
Riversdale Western Cape
South Africa
Send a message via Yahoo to Kobus_Joubert Send a message via Skype™ to Kobus_Joubert
Thanks Mike...In my Cut2D program I select the tool..in this case my 12mm ballnose.. In the toolsetup I use 2000 mm/sec....otherwise Mach3 cuts so slow I will never get anything done.....maybe I need to relook at my Motor tuning in Mach3 and pump up the speed there..cannot remember what it is at the moment.

What does G94 do ....Per Minute Feed....I see it in my file in the beginning.
Reply With Quote
  #15  
Old Fri 20 March 2009, 09:00
Richards
Just call me: Mike
 
South Jordan, UT
United States of America
The G94 code sets the program to use Inches Per Minute.

There's a good reference on G-codes on Wikipedia. It lists many of the codes and their functions.

It seems to me that you might have to make some changes in your Mach 3 setup. On my Shopbot PRT-Alpha, a very common speed while cutting MDF would be about 130mm per second.
Reply With Quote
  #16  
Old Sun 22 March 2009, 05:55
Kobus_Joubert
Just call me: Kobus #6
 
Riversdale Western Cape
South Africa
Send a message via Yahoo to Kobus_Joubert Send a message via Skype™ to Kobus_Joubert
I think it's fixed..... In my cut2D I was setup to use mm/sec....I changed that to mm/min made it 9000 mm/min for the tool and also changed the motortuning in Mach3 from 4000 to 9000.. Did a AIR CUT and all looks OK.

It looks loike Mach3 somehow saw this BIG feedrate comming through, went to the max as setup inthe motor tuning, but somwhere in the middle of the program decides enough is enough and brought the feedrate down. Nowhere in the G-Code is the feedrate changed, but in real live it happened.

Lesson learned....look at feedrates and make sure you understand what you are setting up. mm/sec and mm/min is one big difference.
Reply With Quote
  #17  
Old Sun 22 March 2009, 06:16
Gerald D
Just call me: Gerald (retired)
 
Cape Town
South Africa
Ja, the theory is that Mach3 should have cut the file at max motor speed for all x and y moves......but it didn't.

We had a Mach at one time that was cutting the y axis at half the speed of the x-axis, even though motors and tunings were identical.

On the ShopBot, the displayed speed and the real speed were often far from each other.

These events leave me suspicious of actual feed rates being indicated by our controlling programs.
Reply With Quote
Reply

Register Options Profile Last 1 | 3 | 7 Days Search Today's Posts Mark Forums Read

Thread Tools

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off

Forum Jump


All times are GMT -6. The time now is 06:20.


Powered by vBulletin® Version 3.8.3
Copyright ©2000 - 2023, Jelsoft Enterprises Ltd.