cut2D and Mach3/SmoothStepper

gravirozo
Vectric Wizard
Posts: 1978
Joined: Sat Jan 10, 2009 12:38 am

Re: cut2D and Mach3/SmoothStepper

Post by gravirozo »

hello bisquit man

i'm also mm guy.... my first machine with inch screw.... 4 turn per inch... has microstep, does mean 4x200 one turn on the motor... and four turn of motor one inch...
after i did set this, i shifted to mm... for me this was the simplest...


to determine your axis first you need the direction, and steps...

the velocity-feed is only secondary problem...... and i think no one can give you reasonable value... some machine takes easy 300 ipm, 7500mm per min...
some machine cann take only 40-80 ipm about 1500-2000 mm per min...

start with a low value, start to raise and at the first "slip" you need to set back about 20-30 percent to secure, during a task your machine sure not "slip"

also important your acceleration-decceleration... around ""45 deg"" that is safe... and already a good acceleration... with more acceleration your machine will "jerking" on short distances... like in 3d...

with mach, strongly suggested the cv buffering about 50-80... number of segments the mach precalculate...
also the cv has a settings, where you can determine an angle, on these, and sharper angles, the mach will turn off the cv and slow down to zero, secure the corner sure be sharp... after corner, mach will turn on again the cv...

i hope it helps you...

thanks
viktor

BISCUIT MAN
Posts: 12
Joined: Mon Aug 10, 2009 9:31 am

Re: cut2D and Mach3/SmoothStepper

Post by BISCUIT MAN »

hello metalworkz
>>I see an input of 100mm but no mention of how far the axis actually moved?
the brock move to 100mm point actually.
this image is data When move to X181.245Y173 from x0.y0 on mach3 .(feed rate = 6000 over).

please tel me how to make image(in my PC) in post.

User avatar
ManitobaKeith
Vectric Wizard
Posts: 374
Joined: Sun May 03, 2009 2:06 am
Location: Noble Lake, Manitoba Canada

Re: cut2D and Mach3/SmoothStepper

Post by ManitobaKeith »

I think we are missing the point.
I think the actual problem is that at the very start of the program, at
X=0,Y=0 Z=.600mm all is fine
When it moves to the first location, it moves at a rate of 6000mmPer Minute.
That speed is too fast for BiscuitMan. It should only go at a slower speed.

Biscuitman, please, if this is correct, just let us know, after you get up in the morning.

I tried using BiscuitMan's txt file and travel would go up to 7400 mm PM on my machine (>6000 on his). How does one get it to run slower I think is the question. In an earlier post, I had tried to slow it down to 6 mm Per Minute and it did not slow down, it still went at 7400 in Mach. Viktor, please look at the code and try it - it should have slowed down. IF I am correct, that is what the problem is.

If someone with Cut2D could please tell BiscuitMan how to save the actual code so that he can post it here, I think is the question in the post above mine by BiscuitMan.

I hope this helps, if not, then I am guessing wrong also. This is up to 4 cents worth now :lol:
Keith
It is not only what we do,but also what we do not do,for which we are accountable-Jean Moliere

BISCUIT MAN
Posts: 12
Joined: Mon Aug 10, 2009 9:31 am

Re: cut2D and Mach3/SmoothStepper

Post by BISCUIT MAN »

I tried single BLK on mach.

( Profile 1 )
( Mach2/3 Postprocessor )
N20G00G21G17G90G40G49G80
N30G71
N40T0M06
N50G00G43Z20.000H0 (Z axis = feed rate 600mm/min )
N60S3000M03
N70G94
N80X0.000Y0.000F600.0
N90G00X181.245Y173.093Z6.000(X/Y axis=feed rate 6000mm/min)
(Z axis = feed rate 600mm/min )

In motor tuning(X and Y axis=feed rate 4500mm/min. Z axis=600mm/min)
I did not set numbers (X and Y axis=feed rate 6000 over mm/min)
X axis and Y asis are the problem.
>>That speed is too fast for BiscuitMan. It should only go at a slower speed.
yes too fast, I did not set numbers.

Now, I set check in the button of (Rapid Override Rate(Units/Min))>Setting Alt6 in mach.
and set number (4500).
I think the motor stop rapid(little) to the positon(N90G00X181.245Y173.093),
***This method of resolution is not really.*** I think so.

Now Occurrence of this phenomenon is limited to the data of cut2D.

User avatar
metalworkz
Vectric Wizard
Posts: 2463
Joined: Mon Mar 31, 2008 3:26 am
Model of CNC Machine: SX3 CNC, DIY 24x20 & 48x60 routers
Location: Modesto, California 95358 USA

Re: cut2D and Mach3/SmoothStepper

Post by metalworkz »

Hello,
I think the feeds need to be addressed on the tool definitions to control them. To get the n80 line to have the 600.0 feed rate it must be keyed into the feed rate box. If you want a different feed rate you need to change it there also, and that is under the tool definitions for the tool you are using with the toolpaths. I'm sorry if I am missing all of the details of the problem but this seems to keep being brought up.
Attachments
FeedsSetting.JPG
Best regards,
Wes
wes.spence@comcast.net
Gingery Machines:
Lathe, Horiz. Mill, Shaper, Leaf Brake

gravirozo
Vectric Wizard
Posts: 1978
Joined: Sat Jan 10, 2009 12:38 am

Re: cut2D and Mach3/SmoothStepper

Post by gravirozo »

hello

I COPIED OVER HERE BISCUIT LAST POSTED CODE...


N30G71
N40T0M06
N50G00G43Z20.000H0 (Z axis = feed rate 600mm/min ) HERE'S NO DEFINITION FOR Z FEED... IT IS A RAPID MOVEMENT...
N60S3000M03
N70G94
---------------------------------------------------
N80X0.000Y0.000F600.0

THIS LINE IS CONFUSING... BECAUSE BY PRIOR DEFINITION IT SHOULD BE RAPIDMOVEMENT...
BY POSTPROCESSOR, RAPID TO HOME POSITION... HOW THE FEED DEFINITION GOT HERE?
------------------------------------------------------
N90G00X181.245Y173.093Z6.000(X/Y axis=feed rate 6000mm/min)
(Z axis = feed rate 600mm/min )

THIS LINE RAPID MOVEMENT, DOES MEAN IT WILL MOVE WITH THE MAXIMUM VALUE DEFIFED, UNLESS THE RAPID DEFINED DIFFERENTIALLY... IN MACH...




also controllers are suggested to set all axis for one accelereation, and maximum speed... ie when you set different values, the slower axis will keep back the others, the result the machine by the rapid stops will "jerking"


and here's an other gcode... by biscuit...



N5 (File Name = 30 on Tuesday, August 11, 2009)
N10 (Default Mill Post)
N15 G91.1 incremental mode settings

N20 G0 Z6.0000 rapid to 6.0

N25 M3 start to cut

N30 X154.2181 Y90.9666 due to lack of new definition, the prior definiton works, as this movement is rapid, to the first position where the cut start

N35 Z0.1000 moving still with rapid to level 0.1

N40 G1 Z-4.0000 F50.00 first feed movement with interpolated movement, feed 50 unit per minute

N45 Y1240.9665 F600.00 interpolated movement with feed 600 unit per minute

N50 G0 Z6.0000 from actual position rapid movement to elevation 6.0

N55 X904.2181 Y90.9666 rapid movement to defined position

N60 Z0.0000 rapid movement to zero level

N65 G1 Z-4.0000 F50.00 interpolated movement to level -4.0 (where's the ramping ? ) feed 50 unit per minute..

N70 X154.2181 F600.00 interpolated movement with 600 unit per minute

N75 G0 Z6.0000 rapid movement to level 6.0

N80 X904.2181 rapid movement to x position..

N85 Z0.1000 rapid to level 0.1

N90 G1 Z-4.0000 F50.00 interpolated movement to level -4.0 with 50 unit per minute...



this is a normal g code... i really miss some point what is really wrong here?

if biscuit set his maximum speed for 6000 unit per minute, the rapid will perform 6000 unit per minute.. the code is right... there's no bug...

thanks
viktor

BISCUIT MAN
Posts: 12
Joined: Mon Aug 10, 2009 9:31 am

Re: cut2D and Mach3/SmoothStepper

Post by BISCUIT MAN »

hello gravirozo
Yes, the problem is G00(papido moment)
I understand your pointing out, that's right.
I set max speed 4500 feed rate on motor tuning in mach.
BUT
It is 6000(feed rate) over on G00(papido moment) by the data of cut2d.

It is 4500(feed rate) over on G00(papido moment) by the data of lazyCam.

If someone answers me how to send images to post,
I can see you them.

User avatar
metalworkz
Vectric Wizard
Posts: 2463
Joined: Mon Mar 31, 2008 3:26 am
Model of CNC Machine: SX3 CNC, DIY 24x20 & 48x60 routers
Location: Modesto, California 95358 USA

Re: cut2D and Mach3/SmoothStepper

Post by metalworkz »

Hello Biscuit Man,
With the image you want to send on the monitor, click the Print Screen button of the keyboard(sometimes marked PrtScr on the key) This will copy the image to the system clipboard; then open the windows Paint program(usually Start button, All programs, Accessories,Paint) and once the Paint program is opened select Edit, then paste.
Now the image is loaded and you need to save it as a .jpg so that it can be posted to the forum, but if the file is too large you may have to resize it in the Paint program to get it to post. If you mouse over the file in explorer it will show you the file size. With the file opened in the Paint program select the Image command along the top menu, then Stretch/Skew(Ctrl+W) and reduce both the Horizontal and Vertical settings in the Stretch section and click OK. You can do this more than once if you need to make the image size smaller so it can be posted. I hope this helps you .
Best regards,
Wes
wes.spence@comcast.net
Gingery Machines:
Lathe, Horiz. Mill, Shaper, Leaf Brake

BISCUIT MAN
Posts: 12
Joined: Mon Aug 10, 2009 9:31 am

Re: cut2D and Mach3/SmoothStepper

Post by BISCUIT MAN »

Thanks ,metalworkz
I Found Upload attachment .
and send two images.
Attachments
first rapid speed about 6000 over
first rapid speed about 6000 over
I set 4500(feed rate)
I set 4500(feed rate)

User avatar
metalworkz
Vectric Wizard
Posts: 2463
Joined: Mon Mar 31, 2008 3:26 am
Model of CNC Machine: SX3 CNC, DIY 24x20 & 48x60 routers
Location: Modesto, California 95358 USA

Re: cut2D and Mach3/SmoothStepper

Post by metalworkz »

Hello,
Do you have an .xml profile configuration(setting) file for your machine that is in the Mach3 folder? This file is usually supplied by the company that makes the machine and it configures Mach3 to work properly with that machine. You will load that file when you start the Mach3 loader file, and I am seeing Mach3Mill in the profile display line in your screen shot. Is that the profile file for your machine? If not you need to obtain the profile for the machine and put it in the Mach3 folder for it to be configured correctly. If you have already done that I am sorry for being redundant.
Best regards,
Wes
wes.spence@comcast.net
Gingery Machines:
Lathe, Horiz. Mill, Shaper, Leaf Brake

gravirozo
Vectric Wizard
Posts: 1978
Joined: Sat Jan 10, 2009 12:38 am

Re: cut2D and Mach3/SmoothStepper

Post by gravirozo »

hello

thanks to post these pictures... can you check the z settings?
it looks weird, if your setting is 4500 the mach will not set 6000.... for rapid...

ie on the picture is the x settings...

thanks
viktor

gravirozo
Vectric Wizard
Posts: 1978
Joined: Sat Jan 10, 2009 12:38 am

Re: cut2D and Mach3/SmoothStepper

Post by gravirozo »

hello

on the posted picture, first,,, your machine goes from (home position) and accelerated up to 6000.... my guessing is, some of axis, is set for 6000 or higher...
the three axis are moving simultan...
the cut2d outputted right, with rapid move the tool from zero to the start... cut 2d did not sent command """"feed 6000""" and mach converted the rapid movement to the presetted values, in this case 6000....

also what wes pointed out, the mach user guide says, create a new init file, instead use the originall... in case a fault, still you can "reload" the factory settings...

thanks
viktor

BISCUIT MAN
Posts: 12
Joined: Mon Aug 10, 2009 9:31 am

Re: cut2D and Mach3/SmoothStepper

Post by BISCUIT MAN »

I understand 6000 feed rate when it move rapido(G00)
The End-MILL dose not engrave material ,
so It is no probrem that move rapido 6000 over Obliquely.(4500 * 1.4 =6300)
(Directions = 45dgree)
It is 500 feed rate when the End-MILL engrave material slowly.
(In all directions)
I undestand this in forum,
Everyone ,Thank you very much . :D :P

Post Reply