MechMate CNC Router Forum

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

Reply
 
Thread Tools
  #1  
Old Sat 20 August 2011, 07:47
giggler
Just call me: giggler
 
na
United Kingdom
Wood burn?

hi,

i'm doing a test cut, a collet holder a have drawn to be machined in MDF. The bit I'm using is a four fluted 6mm end mill normally used for metal.

My router can traverse at 10000mm/m (think that's right? i.e. G1 X2440 10000F ; metric) but the acceleration figure I set in turbocnc has a problem with small cuts as it never gets up to speed fast enough.

I was cutting a 17.5mm dia. pocket, 12mm deep done in two pockets of 6mm but the dust comming of isn't all sucked away by my 2HP blower and the bit moves so slow even with the feed set to 5000mm/m as it never seems to have time to speed up and the arc cut is over. On straight lines it seems fine.

I set the acceleration low so that I reduced pressure on the axis motors while testing my machine. My motors are T5 belt driven, ratio 3.75 with a 36tooth gear, module 1. I think this is pretty standard setup from what I've seen on this forum.

What is the realistic acceleration figures I should be using with this open loop, portercable router setup? I have a 7519, that's single speed, i.e. flat out all the time so I figured all I can do is change the bit and speed of cuts.

thanks

dc
Reply With Quote
  #2  
Old Sat 20 August 2011, 08:12
danilom
Just call me: Danilo #64
 
Novi Sad
Serbia
well the feedrate is in gcode but acceleration is done by controller program (like Mach3 and your turbocnc)
10000mm/min is quite a speed for cutting its about 400ipm, I think that some realistic numbers are around 2-5000mm/min. you can use 10000mm/min for rapid moves.
So you sure have a acceleration settings problem. I am not familiar with turbocnc, but try to set acceleration to something about 450mm/min for X and Y and a little slower for Z.
Also try shallower cut with that 6mm endmill as it is 4 flutet it produces much more heat, try 4mm instead, it will also help evacuate chips out of way.
You already know but right endmill to use for wood is 2 fluted carbide.
Reply With Quote
  #3  
Old Sat 20 August 2011, 08:33
giggler
Just call me: giggler
 
na
United Kingdom
Hi danilom.

I will check my acceleration settings, thanks. What HZ figure do you start from? In my configuration setup I put 20Hz in my X/Y start movement and I think 200Hz acceleration. When moving it seems good, but like I said because the small arcs never get up to speed.

I have set my Z axis very low (HZ) and turbocnc seems to limit the rapid traverse (G00 ) to the fastest of the slowest axis which doesn't help, as I only get 2000mm/m (Z maximum) for all axis. So right now until I figure it out, I've been doing rapid traverse using G01 where I can specify feed rate and it'll go up to the configured axis limt.

I used the 6mm endmill as that the largest endmill I had to hand. My dust shoe is also being tested, I had to use a 50mm hose to stop it hitting the legs and allow me to get full movement. It's not perfect but will have to do, MDF just generates dust rather than chips which I think is some of the problem.


attached is the Gcode for my collet holder and dxf, according to dry run it'll take 18mins, which I feel is excessive for such a small item, so perhaps I'm doing something wrong in the cam.

dc
Attached Files
File Type: zip 1-300-8.zip (6.5 KB, 15 views)
Reply With Quote
  #4  
Old Sat 20 August 2011, 08:43
danilom
Just call me: Danilo #64
 
Novi Sad
Serbia
I see F100 and F500 so if you are using metric settings for control it means mm/min and it is too slow. Maybe you are exporting gcode in imperial (inch) setting and control expects it in metric (mm), or something like that?
Reply With Quote
  #5  
Old Sat 20 August 2011, 09:00
giggler
Just call me: giggler
 
na
United Kingdom
Hi danilom.

Yes plunge at 100mm/m and cuts at 500mm/m in MDF. The machine is setup to metric.

It doesn't plunge that often, so I changed the cuts to 5000mm/m and it still isn't any better because it never gets up to anything like that speed around the arcs which make up most of the cuts.

Checked my turbocnc settings,

X/Y: accel. 4000mm/S, start velocity 200Hz, max velocity 20000Hz pulses to step drives. I actually don't know if these are normal but they look ok while traversing and some cuts.

I did a 27mm pocket last week with a 4mm 2flute router bit and it was fine at 10mm depth in MDF but I think I changed the settings since because it was starting if I remember rightly at like 2000Hz (velocity) which made the machine really zippy but loosened the gear grub screws with all the sudden fast moves.

dc
Reply With Quote
  #6  
Old Sat 20 August 2011, 09:14
danilom
Just call me: Danilo #64
 
Novi Sad
Serbia
From TurboCNC manual:
Accel: the maximum acceleration of the step pulse train or phases that are sent to the driver measured in cycles per second per second. This is purely electronic, and is converted to motion by the motor.

some parameters I found on net:

Acceleration=2000.000000000000
StartSpeed=150.000000000000
MaxSpeed=350.000000000000
Fast_Jog=350.000000000000
Slow_Jog=50.000000000000

So the acceleration is measure of number of pulses per second and this 2000Hz setting seems rather ok.
But...
If you have microstep drive it accepts let say 10 microstep, and using a 200 steps per rotation its 2000 steps to turn motor one turn.
Using module 1 and 36 tooth pinion its 113.097 mm per turn but with 3.75 reduction its
30.16mm of real movement. So with 2000hz I think the acceleration is ~30mm/sec if using 10 microstep drive and 1800mm/min , So in my case realistic setting would be 500hz and it would equate to 450mm I am using.
Reply With Quote
  #7  
Old Sat 20 August 2011, 09:17
danilom
Just call me: Danilo #64
 
Novi Sad
Serbia
Always test settings first using aircuts or foam!
Reply With Quote
  #8  
Old Sat 20 August 2011, 09:34
giggler
Just call me: giggler
 
na
United Kingdom
danilom,

Always test settings first using aircuts or foam! Yes I should have for sure...

You are correct, the X/Y drives are setup with 10microsteps and you've got more information than I have on the module1 setup. Actually I have some other questions regarding this I'll post in another thread.

I think the StartSpeed is a problem, mine is at 200hz, with a small arc, it doesn't get up to a reasonable cut speed.

dc
Reply With Quote
  #9  
Old Sat 20 August 2011, 09:40
danilom
Just call me: Danilo #64
 
Novi Sad
Serbia
Module 1 has spacing of PI which is

π = 3.141592653589793238462643383279502884197169399375 10...

36 tooth * pi = 1 revolution
divide by 3.75 (your reduction) to get distance traveled with one motor rev.



-Problem might be only in accel I think. but check this from turbocnc manual

Scale: is the distance or angle that the axis moves for a single step pulse or phase change. The units can be in inches, millimeters or decimal degrees, depending on axis motion, and the system of measurement in use. A custom calculator is accessable by clicking on 'Calc, or pressing 'c'.

Start vel: is the maximum starting / stopping velocity that will be used by TurboCNC for this axis. Lower values will often be used for interpolated moves. This is measured in cycles per second, and converted to a distance or angular measurement using Scale and displayed below as the Start Speed.

read further here>
http://www.dakeng.com/man/turbocnc.html

Last edited by danilom; Sat 20 August 2011 at 09:43..
Reply With Quote
  #10  
Old Sat 20 August 2011, 10:25
giggler
Just call me: giggler
 
na
United Kingdom
hi danilom.

you inadvertently solved a step problem I've had since last week

i used the mechmate excel worksheet to calc. my max feed based upon the belts, pully ratio and pinon gear used. as I use metric it was helpful to have around figure and sure enough for my setup which you already know, the sheet shows a step of 0.015mm but i didn't notice the rounding error.

fast forward to machine testing, aligned with a physical 2m rule, it always under travelled logically unless I increased the step figure which i figured out to around 0.0157675mm/step. However your equations got me thinking, and I did some basic math , turns out that 0.015mm should actually be 0.0150796447372... At first I thought it was backlash and was gonna post about it later but then because the error was constant in any direction I thought I'd look into it later.

i'm off 2 try it now Will also test my 4mm 2flute wood bit, but change the gcode to machine it slightly different since the bit depth is only to 10mm which is why i picked the 6mm bit.

thanks

dc
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

Similar Threads
Thread Thread Starter Forum Replies Last Post
cnc wood lathe javeria Miscellaneous / General / Whatever / Catchall 5 Fri 11 March 2011 08:12
Critical wood movement Art Cutting various materials - bit selection, feeds, speeds 10 Mon 12 April 2010 12:38
Extruded wood? - actually a composite of wood and recycled plastic . . . . . Gerald D Miscellaneous / General / Whatever / Catchall 2 Wed 02 July 2008 22:51
Wood plague ekdenton The Show Room 3 Fri 23 May 2008 10:44
Wood carving machine Yuriy Kholodov Archives 5 Mon 12 March 2007 21:03


All times are GMT -6. The time now is 12:59.


Powered by vBulletin® Version 3.8.3
Copyright ©2000 - 2018, Jelsoft Enterprises Ltd.