Machsupport Forum

Mach Discussion => General Mach Discussion => Topic started by: halftonner on December 31, 2014, 07:31:39 PM

Title: Mach 3 & Denford Orac spindle speed headache!!
Post by: halftonner on December 31, 2014, 07:31:39 PM
Hi all,

 recently obtained a Denford Orac lathe and PC running Mach 3 ... It came from a firm that produced items in aluminium and so spindle speed wasn't an issue (nor was the ability to reverse the spindle) - and so I've completed the task (as all the break out boards and motor control was in situe, just needed the additional wiring to make it operational)

The problem I've run into is trying to do constant surface speed - mathematically it is always incorrect if my understanding of G-coding is correct.

G96 = constant surface speed in units per minute ... Mach 3 is running in mm as specified in the G-Code 'header', so my understanding is that G96 S20 should give a surface speed of 20m per minute however, when working out Speed (from Mach 3 DRO) in rpm x diameter x pi = something nowhere near the supposed surface speed!!!

The Orac instructions claim that the spindle can rotate upto 2000rpm, but this turns out to be an impossibility (unless I'm missing something very obvious) as the motor is rated at 1400 rpm, and the belt drive gives a step down speed of approx 0.6, so the max spindle speed can only ever be 840 rpm!! - Though the pulley ratio is irrelevant to one extent as the speed / timing / index sensors are on the spindle, so should always give the true spindle rpm?

Anyway I digress - I added a screen shot of Mach3 running in constant surface speed, and I'll let you do the maths and see if I'm missing something, or if there is indeed something wrong.

Please help as it's been 3 days of headache and measuring and re measuring and taking the belt drive off to measure pulley diameters and circumfrences and maths and countless scraps of paper calculations and I seem to be no further forward :(

(http://www.tep.me.uk/Orac/G96Speedissue1.png)
Title: Re: Mach 3 & Denford Orac spindle speed headache!!
Post by: Overloaded on December 31, 2014, 09:08:51 PM
Your screen is calculating in INCHES. (FPM)
Do your math and divide by 12 instead of 1000 (MPM)and you'll see.
It comes out much closer.
You must have a conflict in UNITS chosen.
Russ
Title: Re: Mach 3 & Denford Orac spindle speed headache!!
Post by: angel tech on January 01, 2015, 05:39:41 AM
to get 2000 rpm you'll need to run the inverter at 100hz or more.
Title: Re: Mach 3 & Denford Orac spindle speed headache!!
Post by: halftonner on January 01, 2015, 06:36:37 AM
with regards to the units issue mentioned... if I set the feed rate to be 10 units / min, the slides move at 10mm / min (I've checked and measured. Also when typing in the code either via a loaded program or via the raw command line on mach3 the slides travel that given distance in mm... so apart from wanting to change the 'label' on the screen to be feed rate mm/min all seems fine - unless something had been set up wrongly by the company that used it (though I've seen the code and the parts produced and they are all done in mm and match the specifications)

with regards to the inverter frequency - the motor has a rating of 50Hz - so surely the investor needs setting to that too? OR is it the 1400rpm comes from when running the motor on 50Hz, thus if I feed the motor 100Hz it would then rotate at 2800rpm (thus giving an approx spindle max of 2000rpm). did the original Orac motor inverter drive feed 100Hz to the motor?
Title: Re: Mach 3 & Denford Orac spindle speed headache!!
Post by: angel tech on January 01, 2015, 06:42:15 AM
yes and yes.

The motor will run at 1425 rpm at 50hz, so increasing the frequency of the inverter you increase the speed of the motor.

The original inverter supplied with the orac would be set to  0-100hz.
Title: Re: Mach 3 & Denford Orac spindle speed headache!!
Post by: Hood on January 01, 2015, 08:38:42 AM
One point to remember is that the speed set in spindle pulleys can affect the displayed value.
Or at least that is the case when using an external controller, cant remember if its the same with the parallel port as it has been a long time since I used one.

So anyway if you have a max rpm of 2000 you should set that in Spindle Pulleys so that the correct RPM will be displayed.
Hood
Title: Re: Mach 3 & Denford Orac spindle speed headache!!
Post by: Overloaded on January 01, 2015, 08:41:10 AM
Check your Native Units setting as that is what seems to determine which divisor is used.
Both work fine here, but need to shut down and restart after changing.
Russ
HNY !
Title: Re: Mach 3 & Denford Orac spindle speed headache!!
Post by: halftonner on January 01, 2015, 08:50:59 AM
right, tried the inverter frequency, and it threw a hissy fit and had an error displayed (I did look it up and it was to do with current ratings. ... if it helps for this part of the question,the motor drive inverter is a Siemens G110

done the native units, and that works fine now for the feed label.

so, still no joy on getting the spindle rpm up to 2000 as claimed (partially as the motor is rated at 1400rpm and the inverter drive doesn't want to output more than 50hz atm) and still no joy on the css (g96) code yet - it still seems to misbehave, as at g96 s1 the motor runs at full tilt and warning comes up too fast for pulley. if I do g96 s0.9 it complains it's too slow for the pulley and won't revolve at all.

sorry for the loads of questions, bit I've struggled for the last few days on this, and decided it's time to ask for help :)
Title: Re: Mach 3 & Denford Orac spindle speed headache!!
Post by: angel tech on January 01, 2015, 09:04:28 AM
often with inverters there are several parameters that need to be changed to go above the default settings.
Title: Re: Mach 3 & Denford Orac spindle speed headache!!
Post by: Hood on January 01, 2015, 09:07:54 AM
Ok first thing to say is be aware CSS doesnt work too great in Mach3, never has, never will.

If in Feed Per Min mode (G94) then it kind of works but to my mind CSS and G94 is not really using things as they should be, you will be keeping the surface speed constant but your feedrate will also stay constant so the chipload will increase or decrease as the spindle speed alters.

In G95 (Feed per Rev) it doesnt work as all it does is keep the feedrate constant to what it was at the start of the commanded move, ie it basically sees it as a G94 feed and keeps it at that.


Now your messages, probably you see the Too Fast one as you are commanding a CSS and a X move which will mean that your spindle will need to rotate faster than it is set in Spindle pulleys.
You can limit the max spindle speed from the code with a G48.
For example
G96 S200  (this will set your surface speed to 200 units per min)
G48s1400  (this will ensure that the max RPM never exceeds 1400)

Hood
Title: Re: Mach 3 & Denford Orac spindle speed headache!!
Post by: halftonner on January 01, 2015, 09:13:39 AM
ok, I'll have to study the inverter manual again...

and reading between the lines about css and feed rate per rev are best avoided in mach3 - I'm not too worried as I can manually program them to keep chip load and spindle speed approx constant (just need to keep a calculator to hand) :)

BTW happy new year to all, and thank you again for all the help :)
Title: Re: Mach 3 & Denford Orac spindle speed headache!!
Post by: Hood on January 01, 2015, 09:28:47 AM
Not sure if it will be of any use but attached is a spreadsheet I made up for myself.
Hood
Title: Re: Mach 3 & Denford Orac spindle speed headache!!
Post by: halftonner on January 02, 2015, 09:12:51 AM
question about constant surface speed... I've just read elsewhere that G96 relates to a constant RPM....

eg
X10
G96 S1000

would give a spindle speed of 1000rpm at the current X tool position 10mm diameter .. then as the tool comes in closer the RPM increases to max... if the tool moves further away from X10 (ie X15) the spindle will slow down below 1000rpm

have I interpreted this correctly or is the S followed by a surface metres / min

Btw, HOOD, thanks for the calculator xls sheet - it will come in handy :)
Title: Re: Mach 3 & Denford Orac spindle speed headache!!
Post by: Hood on January 02, 2015, 09:21:43 AM
G96S1000 would give you 31,837 RPM at X 10mm dia.

BTW not sure if the spreadsheet opens part way down with you. I just opened it to calc the rpm and it was sitting with the No of Teeth box uppermost, if you scroll up yuou will see the VC, Dia etc fields.


G96 is Constant Surface Speed
G97 is Constant Spindle Speed

Hood
Title: Re: Mach 3 & Denford Orac spindle speed headache!!
Post by: halftonner on January 02, 2015, 09:29:23 AM
shame about the CSS idea... the website I read it from was mis-informing me then :(
Title: Re: Mach 3 & Denford Orac spindle speed headache!!
Post by: Hood on January 02, 2015, 09:33:19 AM
Not sure what you are meaning but CSS will vary the spindle speed depending on the Dia. What was wrong in your post above was that G96 was Constant RPM, that is G97.

So to summarise if you call a G96S200 the RPM will go to whatever is required to give a surface speed of 200 at the diameter you currently are at. If you move to a smaller dia the spindle will increase in RPM and move to a bigger dia and it will decrease.
Hood
Title: Re: Mach 3 & Denford Orac spindle speed headache!!
Post by: halftonner on January 02, 2015, 10:08:14 AM
Head to:

http://www.hsmworks.com/docs/cncbook/en/#Ch08_CuttingSpeedsAndFeeds

and look at table 8.9

This is where i got the suggestion that G96 gives constant surface speed

Sorry if I'm sounding idiotic, but I've read and re-read about CSS, and it makes sense on paper, but in reality it doesn't quite behave ...

Hood, you mention that CSS is in units per minute, so if I have set the code to run in mm then should I multiply out the Surface Metres / Min given in cutting tables to become Surface mm / min for the G-Code?
Title: Re: Mach 3 & Denford Orac spindle speed headache!!
Post by: Hood on January 02, 2015, 10:17:30 AM
The Units in CSS are either Meters or Feet depending on whether your code is metric or Imperial.

So if metric the S word after a G96 will be meters, so G96S200 will be a surface speed of 200m/min.
In your previous post you said that the site you had looked at was saying G96 was constant RPM, it is not. G97 is constant RPM, G96 is constant surface speed.

If you call G97S200 it will rotate the spindle at 200rpm and it will not vary if you vary the X axis and it will not matter what the current X axis value is when you call the G97S200.

If you call G96S200 it will start the spindle rotating, what the RPM will be will be dependent on the current X axis position. As the X axis moves the RPM will follow to keep the surface speed constant, so decrease the dia and the spindle speed will increase, Increase the Dia and it will slow..

Hood
Title: Re: Mach 3 & Denford Orac spindle speed headache!!
Post by: Overloaded on January 02, 2015, 10:26:35 AM
That link is not correct as far as Mach is concerned.
It says G96 actually sets the RPM. ... if I see it right.

 Russ
Title: Re: Mach 3 & Denford Orac spindle speed headache!!
Post by: halftonner on January 02, 2015, 10:35:19 AM
Overloaded - I am agreeing with you ... but I've ended up getting myself confused .... :(

G96 = CSS
G97 = Constant RPM

sorted:  :)

Hood - one last question for your spreadsheet calculator: is the feed per tooth the cutting depth on that pass?
If not, where would I find the data to enter into that cell?
Title: Re: Mach 3 & Denford Orac spindle speed headache!!
Post by: Overloaded on January 02, 2015, 10:36:33 AM
Here is some more info on the subject:
http://www.cnccookbook.com/CCCNCGCodeG96ConstantSurfaceSpeed.htm
although, Hood has it pretty well covered .... as usual.  :)

Russ
Title: Re: Mach 3 & Denford Orac spindle speed headache!!
Post by: Hood on January 02, 2015, 10:43:09 AM
The Teeth and Feed per tooth entries are really meant for milling cutters. The manufacturers will give a feed per tooth and if you are using a lathe then the "tooth" will be 1, if for example you have a 4 flute milling cutter and the feed per tooth is 0.2 then that would mean you actually move the cutter at 0.8mm/rev.



Hood
Title: Re: Mach 3 & Denford Orac spindle speed headache!!
Post by: halftonner on January 02, 2015, 10:57:14 AM
so is there a recommended feed per tooth for carbide bits and likewise for HSS tools?
I know that the lathe tool has in effect only 1 cutting tooth
Title: Re: Mach 3 & Denford Orac spindle speed headache!!
Post by: Hood on January 02, 2015, 01:11:58 PM
Most carbide inserts for lathe tools will have the vc  (suface speed) and fz (feed per tooth per rev) on the box.
Likewise carbide inserts for milling cutters will also usually have this info.
For carbide and even HSS milling cutters you should find info on the manufacturers web site.

As an example here is the info for the powdered metal cutters I use for stainless.
http://www.cutwel.co.uk/FileDepository/%5CProductId%20-%2083/Cutting%20Data%20GA942.pdf

YG give you a bit more info than normal as they give you the rpm and feed per min and as such save you having to calculate them.

Hood
Title: Re: Mach 3 & Denford Orac spindle speed headache!!
Post by: RICH on January 03, 2015, 07:11:11 PM
This document provides a lot of info on speeds and feeds.

http://www.machsupport.com/forum/index.php/topic,20045.msg138970.html#msg138970

RICH