Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: Shaggy on September 13, 2016, 06:02:26 PM
-
Hi guys,
Im into aluminium engraving. I must engrave a lots of letters (words) on big aluminium plate and some of letters are very far from each other.
My question is:
Is there any option in Mach3 where I can set up that my CNC machine go faster when it is above material and slower when it is in material ?
For example I want 1200 mm/s when my mill is into material I want to engrave and 2400 mm/s when it is above material (mill is going to another letter).
Whit that I would be able to reduce my time a lot.
Thank you !
-
Yes! G0 and G1. G0 runs at the maximum configured motor speed and would be used when the tool is above the material. Then G1 is used for the cutting moves and can be programmed for a different speed with the "F" word parameter. That is actually what these two commands were designed for. G0 for rapid moves and G1 for cutting moves.
Hope that makes sense.
Stephen "Highspeed" Kruse
-
What is the maximum speed your machine is configured for? It may be going slower simply because it cannot go any faster :)
Motor Tuning -> Speed for X & Y axes.
As mentioned above, is your G-Code using both G0 & G1 moves?
-
Well guys thanks for fast replay's ! :)
At the moment my Velocity is set to 500 in MACH3.
I don't know what is maximum speed my machine can go, but it certainly can go faster than that (500).
Where do I set G0 and G1 parameters ?
I suppose if G1 is used for cutting moves it can be set in Motor Tuning under Velocity tab.
But where do I set G2 speed ?
Cheers
-
If its at 500 then that is your current max speed with ANY code, that does not mean it is all it can do though, who set that speed?
To go higher will need testing and tweaking unless you know for a fact that it can do it, not hard just tedious ;)
If you look at your G-Code file, you should see lines beginning with G0, G1, G2 etc these are the moves, G0 is a rapid and never used for cutting, G1 is a cutting move - straight at a feed speed commanded by the F parameter on or near that line, G2 is clockwise circular cutting again with an F parameter maybe and so on, these are all documented - Google Mach3 G codes and you will get a document that explains it all.
Now, there is no point in the code asking for a speed of say F1000 if your machine is pegged at 500 - it will be limited to 500 for cutting OR rapids.
To increase the speed you change the settings in motor tuning, increase in small amounts say 100 at a time, save it then jog the machine at full rapid (shift & jog) if it screams you have gone too fast and the motors are throwing in the towel, if ok then advance some more, at some stage it WILL give up, at this point you need to back off maybe 20% and start testing for lost steps - this will cause circles to come out square and other lovely cock-ups :)
Its an art to get right as every machine is totally different, but can be done, just make sure you note what you are doing.
Once you have found the sweet spot, set the acceleration to 1/10 of the speed and start testing again for lost steps etc.
Definitely get the book on G-codes though, there is also a smaller on on M-Codes :)
Also a little more info on the machine would be good
-
G0 and G1 are modal commands, meaning that once set it is the active mode until a different modal command is set. As an example:
G0 X0 Y0 Z0
X1
Y2
G1 Z-0.5 F50
X4 Y5 F600
X3 Y7
In this rather basic program, the machine is set to rapid movements (G0) and positions the tool at zero for all axes, then moves (still at rapid movement) the X Axis to 1 followed by a movement of the Y axis to 2. (These two moves can be combined into one line and the tool would then traverse at a diagonal line from 0,0 to 1,2 rather than a straight move along the X axis and a seperate move on the Y axis. Next, a cutting move (G1) is made on the Z axis to -0.5 at a feed rate of 50 followed two cutting moves (still in G1 mode) at a feed rate of 600 to various points on the X and Y axis. These last two moves are diagonal moves since the X and Y values are on the same line and the feed rate (F600) is set until changed by a different F word so both of the last two moves are made at a feed rate of 600.
In Motor Tuning, adjust the Velocity to the speed at which your machine is capable of running RELIABLY. This velocity is what is used for G0 moves. You'll also need to adjust acceleration accordingly to get smooth starts/stops as well as keeping it high enough so that corners don't become rounded.
As shown above, G1 moves are made at a speed determined by a feed rate command. This can be set with F followed by a number or you can manually set it through the feed rate controls on the Mach 3 screen. However, if you set it through the screen controls it can be altered by the program if an F command is encountered. But again, to really summarize:
G0 - Rapid move at the velocity set in Motor Tuning
G1 - Cutting move at the currently set (via program or screen) feed rate.
Hope that makes sense.
Highspeed
-
G0 and G1 are modal commands, meaning that once set it is the active mode until a different modal command is set. As an example:
G0 X0 Y0 Z0
X1
Y2
G1 Z-0.5 F50
X4 Y5 F600
X3 Y7
In this rather basic program, the machine is set to rapid movements (G0) and positions the tool at zero for all axes, then moves (still at rapid movement) the X Axis to 1 followed by a movement of the Y axis to 2. (These two moves can be combined into one line and the tool would then traverse at a diagonal line from 0,0 to 1,2 rather than a straight move along the X axis and a seperate move on the Y axis. Next, a cutting move (G1) is made on the Z axis to -0.5 at a feed rate of 50 followed two cutting moves (still in G1 mode) at a feed rate of 600 to various points on the X and Y axis. These last two moves are diagonal moves since the X and Y values are on the same line and the feed rate (F600) is set until changed by a different F word so both of the last two moves are made at a feed rate of 600.
In Motor Tuning, adjust the Velocity to the speed at which your machine is capable of running RELIABLY. This velocity is what is used for G0 moves. You'll also need to adjust acceleration accordingly to get smooth starts/stops as well as keeping it high enough so that corners don't become rounded.
As shown above, G1 moves are made at a speed determined by a feed rate command. This can be set with F followed by a number or you can manually set it through the feed rate controls on the Mach 3 screen. However, if you set it through the screen controls it can be altered by the program if an F command is encountered. But again, to really summarize:
G0 - Rapid move at the velocity set in Motor Tuning
G1 - Cutting move at the currently set (via program or screen) feed rate.
Hope that makes sense.
Highspeed
It makes perfectly sense. Thank you !
If i get it right the procedure is next.
I want my machine to move 500 mm per m when it is in material and i set that in mach 3 - motor and tuning - velocity tab.
I want my machine to go 1000 mm per m when it is not in material and for that I should go into G-Code with Notepad (for example) and change all G1 F's from 500 to 1000 (for example).
And that will make my machine goes 500 mm per m when it is in material and 1000 mm per m when it is above material. Correct me if I am wrong.
-
Not quite correct but you have the right idea.
I want my machine to move 500 mm per m when it is in material and i set that in mach 3 - motor and tuning - velocity tab.
You set that in Gcode with the F### command.
I want my machine to go 1000 mm per m when it is not in material and for that I should go into G-Code with Notepad (for example) and change all G1 F's from 500 to 1000 (for example).
You set that in Motor Tuning with Velocity.
Tweakie.
-
Not quite correct but you have the right idea.
I want my machine to move 500 mm per m when it is in material and i set that in mach 3 - motor and tuning - velocity tab.
You set that in Gcode with the F### command.
I want my machine to go 1000 mm per m when it is not in material and for that I should go into G-Code with Notepad (for example) and change all G1 F's from 500 to 1000 (for example).
You set that in Motor Tuning with Velocity.
Tweakie.
My mistake. I'll try that right away.
Usualy I make G code with ArtCAM.
Is there any software that can change G00 G01 speeds automatically instead of me doing it manually in Notepad ?
-
Usualy I make G code with ArtCAM.
Is there any software that can change G00 G01 speeds automatically instead of me doing it manually in Notepad ?
The Gcode G00 / G01 moves are usually automatically taken care of by the post processor used in ArtCam.
Are you using their Mach2 post processor ?
Tweakie.
-
Usualy I make G code with ArtCAM.
Is there any software that can change G00 G01 speeds automatically instead of me doing it manually in Notepad ?
The Gcode G00 / G01 moves are usually automatically taken care of by the post processor used in ArtCam.
Are you using a Mach3 post processor ?
Tweakie.
I don't know what exactly do you mean by ''post processor''.
I use ArtCAM to generate G code and than I use MACH 3 to transfer it to machine. I just upload saved code in MACH 3 and start the job.
-
I don't know ArtCam but the post-processor is a part of the program that adjusts the code generated to suit various machines - G-Code has many different flavours and needs tweaking to suit the hardware.
It is usually an option at save time or in the preferences somewhere - you need a processor that lists Mach3 etc, its probably using a generic one which sort of works most times.
The feed and speed are usually set in the CAM stage of the job and then passed through the processor as G and F parameters etc.
-
Thank you guys for help!
I get it all.
Where was the problem?! Well since I'm pretty new to CNC processing I didn't saw that there is in ArtCAM under ''Profiling tool'' menu a tab where you can set Feed rate , Plunge rate, RPM and so on.
I was doing a mistake by leaving all the time default value for 2 mm End mill which was 13 mm/sec. That default value (13 mm/sec) was too fast for aluminium engraving so instead of changing Feed rate in ArtCAM I was limiting my machine speed in Mach 3 under tab ''Motor and tuning''. That resulted with a enormous waste of time in every one of my jobs.
Now I set my Mach 3 machine speed to 1500 mm/min and that allows fast movement over the material, but when mill touch the material than it slows down to a speed I've entered in ArtCAM under ''Profiling tool'' values.
Next thing I need to do is to calculate feed rates and RPM for my 2 mm carbide End mill and input that settings in ArtCAM.
This was pretty simple problem to solve but for every other confused person out there I tried to explain the best I could where I was mistaken.
Cheers !
-
I can get you some figures if you let me know your spindle power and what type of tool - 1flute or two flute etc.
Or you can look in to a program called HSMAdvisor its great for speeds and feeds but you will need to know how to set it for a small machine as it assumes industry size stuff :)
Once set correctly, the motor tuning never really gets looked at again, unless you alter the machine etc.
Is there a tool library feature in ArtCam - this is where i would set my feeds for each tool/material combination then its just a simple matter to choose the tool when doing the CAM and you always get the right speed settings etc. :)
I use 2m single flute carbide a lot in aluminium and on my machine i use 24,000rpm, 370mm/min feed, 1mm depth max, 0.59mm width max and it will run this all day.
You can tune differently though as it will also run a 5mm cut depth but only at a max of 0.1mm engagement - great for finish passes.
-
There is lot of "stuff" out there on speeds and feeds.
Have a look at the PDF in the link below to get grounded on the subject.
http://www.machsupport.com/forum/index.php/topic,20045.msg138970.html#msg138970
RICH
-
I can get you some figures if you let me know your spindle power and what type of tool - 1flute or two flute etc.
Or you can look in to a program called HSMAdvisor its great for speeds and feeds but you will need to know how to set it for a small machine as it assumes industry size stuff :)
Once set correctly, the motor tuning never really gets looked at again, unless you alter the machine etc.
Is there a tool library feature in ArtCam - this is where i would set my feeds for each tool/material combination then its just a simple matter to choose the tool when doing the CAM and you always get the right speed settings etc. :)
I use 2m single flute carbide a lot in aluminium and on my machine i use 24,000rpm, 370mm/min feed, 1mm depth max, 0.59mm width max and it will run this all day.
You can tune differently though as it will also run a 5mm cut depth but only at a max of 0.1mm engagement - great for finish passes.
I use 1 Flute 2 mm end mill from sorotec - http://www.sorotec.de/shop/Cutting-Tools/END-MILLS/END-Mill-ALU-412/End-Mill-Z1--2-0mm-SL-5-ALU.html
There is tool library in ArtCAM and setting parameters for each tool is my next step.
My engraving does not go deeper than 0,5 mm so till now i did 2 step down's of 0,25 mm each.
When you say 1 mm max depth do you make that depth in single pass or you make it in a couple of passes (step downs) ?
@RICH
Thank you for link !
-
Depends on the process - if slotting then no, multiple step-downs, if side-milling then yes but only with engagement of 0.59mm max - you have to balance one with the other especially at this tool size.
I think i go to 0.3mm step-down if slotting (cutting full-width) but keep the speed/feed rates.
I use "Alu-Power" single-flute YG carbide from CutWell ltd