Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: marcel beaudry on March 20, 2009, 09:41:04 PM
-
Iis there a way for the wizzards to be changed from units per min to units per rev
I work with very small carbide end mills and even with a feed of .01 unit per min the end breaks i need to cut at 6000 revolutions .0002 per tooth.
Thank you for your time
Marcel Beaudry
-
Hi, Marcel
If your "Step's Per." value's are More than 10,000 in Motor Tuning, You should be able to move as slow as 0.0001 in per min. F0.0001 value.
Hears a Screen.set that shows the F setting, Now that is Slo--------w.
Chip
-
Am I missing something here, or is my maths all wrong.
If you want your tool to advance by 0.0002 (I assume this is the tooth dimension) on a two flute cutter, then at 6000 rpm the feed should be 2.4 units per minute - whether inches or mm does not matter - or am I way out.
In answer to the post, yes, it is possible to change the feed from units per min to units per rev, but this will involve you changing the GCode.
This might not be as difficult as it sounds, with the search and replace facility, but depending on who wrote the wizards, whether he (or she) would be willing to sit down and add it in would be up to them.
I think, however, if you work out accurately what movement you need, if you are fairly accurate with your spindle speed, and it does not vary overmuch (as in Constant Surface Speed work), then using this as a units per minute feed should not make any difference.
-
Thank you for your replies
All my machinist life as been working in thousands per tooth, on manual machines,you can feel the cutter . I have to wrap my mind on cnc milling of letting the machine go on it's own,and using very small carbide end mills .125 or less ,it is quite a challenge .
And working with titanium and manganese bronze does not help .
Well i always like a challenge and this is it.
Marcel Beaudry
-
Hello Chip
Even if i use the mpg to jog only the units per min works , the unit per revolution does not show anything.
Hope this helps
Marcel
-
Hi, Marcel
Post a copy of your Mach3Mill.xml file so I can take a look at your setup. I've sent you a PM message.
Chip
-
Hi, Marcel
Enjoyed the conversation with you today, Now that I have a better understanding of your setup.
I was thinking you couldn't get your F speeds slow enough or your Steps Per wasn't allowing a small enough step move value.
The best solution is to use/make a chart for your cutters and establish a F speed for the material and cutter size's your using in unit's per minute.
I don't think there is a practical way to use G95 with your current setup.
There might be a way if your Spindle was setup as a lathe is setup, But that would require allot of re-configuring work
Thanks, Chip
-
Hey Marcel, These links may help.
http://www.whitney-tool.com/html/calculatorSpeedFeed.html
http://machine-tools.netfirms.com/17_Calculating%20SpeedFeed_Milling.htm
http://www.robbjack.com/html/body_calc.html
http://www.custompartnet.com/calculator/milling-speed-and-feed
Hope that helps,
Brett
-
Chip/Marcel
Just wondering why G95 cant be used, do you not have spindle feedback?
Hood
-
Hi, Hood
He has spindle feedback and is going to post his xml file later today and will need some guidance in configuring the setup.
Chip
-
Hello Chip
I too like the phone conversation.
Maybe have another soon thanks for the help,sent you a xml on your private email.
Marcel
-
Hi, Marcel
I'll take a look at the xml file.
Any Time, Chip
-
Chip i sent you the xml to at
Your email
Marcel
-
Hello to all
Made a test today when i go to manual screen input g20g95 m04 s2000 x-1f.001it does what i iimput but the display screen still shows in unit/min not in unit/rev
hope this helps
Marcel
-
Are you using the standard screen? Go into Screen4 and edit the DRO to feedrate then it will show what you want. The Feedrate DRO that is on screen however will already show that and I dont have a clue why there is the extra DRO there to show FPR as obviously its not looking at the correct info. The IPR will always be what you have in your code however the actual feed per minute will depend on the True spindle speed when you actually start your G95 move. For exaple if your code calls for 2000rpm and feed of 0.1IPR and the True spindle speed was reported as 2000 the FPM would be 200, however if your true spindle speed was actually only 1000rpm then the Feed DRO would still show 0.1 but the FPM would be showing only 100.
Oh and also if you are putting feedrates of 4 digits after the decimal point then you will need to edit the format string to suit, ie %1.4f
Hood
-
Hello Hood
You will have to explain more in detail how i can change my screen 4 as i am not to computer literate ,but can follow instructions step by step.
My rpm is really what is shown on the dro if i imput 6000 rpm it goes 6000 rpm if i imput 300 it goes at 300.
Thank you for your time
Marcel
-
Marcel, I have sent you a personal message.
Brett
-
Not sure if Brett has sorted you out or not, thats the problem with doing the PM thing ;)
If he hasnt then all you do is go to your Mach3 folder and double click on Screen4.exe. When that opens open the screenset you are using from the File menu then Open. If its the standard mill one it will be 1024.set, once thats open just double click on the DRO for Feed per Rev and change it from the dropdown box to Feedrate, then in the Format string change to a 4 after the decimal point, then thats you done, just save and exit You might want to however save the set as a custom one, if so then instead of save use Save As option and name it what you want. When you next open Mach go to View menu the Screens and browse and load the screenset.
As said previously it will only really display the feedrate set in the code, it wont distinguish between a G94 or G95 move.
Hood
-
Hi, All
Hears Marcel's xml, It uses PWM spindle cont.
Chip
-
There is no Index pulse set up in that XML so no way for Mach to know what the spindle is doing and thus no way it can do a G95 move.
Hood
-
Hi, Hood
Will he need to add a separate spindle pickup or is there a way to use the pwm info. ?
Chip
-
As far as I know it will need a single pulse per rev input. What Mach does at the moment as far as a G95 move with no feedback is throw a message then go on its merry way and just assumes that the spindle is turning at the commanded rate. To my mind this is totally wrong, it should throw the message and then do nothing. The way it is at the moment your spindle may not have switched on and Mach will plough the tool into the stock regardless.
Hood
-
Hello to all
Chip found the problem the spindle as no spindle feedback .
Thanks again to all the people who have help me.
Marcel Beaudry ;D