Hi,

My first post. I'm a CNC machinist from Finland. At work I use VMC and as an hobby I have converted Opti BF 20 Vario to CNC with my friend Andy55.

Andy55 has built our Geckodrive stepper electronics and take' s care of the
computer things also. We use EMC2 control. I take care of the mechanics.
Few pics of the current state of the project below. There's actually only
column and base left from the original machine anymore...

You can watch a short video of the machine on action from here:

http://www.anderswallin.net/2007/07/opti-bf20-in-action/

Put enough volume, sounds are good!!!
I will post more videos later. Rapids are painfully slow, put with small steppers
it's better to have low acceleration/ top speed and have good reliability.
I have stalled steppers too many times with higher rapids.
DC servo's are coming...

Little bit of history about this project:

This project started about five years ago and was simple low cost CNC project
at the beginning. Only handwheel' s were replaced with stepper motors at the
beginning and I made wooden bench for the machine. We were looking for a
machine with 500 mm X- travel, but Opti BF20L, Grizzly G0519 or similar low cost machines were not available then and we could not afford Wabeco F1210 E.

When you learn more about CNC machining and want to drive faster and faster, you have to start tuning your machine! First part to replace was standard 600W DC spindle motor since I run out of spindle power all the time. I burned couple control board fuses and finally when the spindle speed control board itself burned instead of fuses, change had to be done. Standard spindle motor was replaced with 0,75 kW three-phase induction motor and variable-frequency drive (VFD).

Whow! Hobby use?

Nice!

JMI will post more pictures later, but there are some pics and text about our efforts on my blog:

the stock DC motor on the mill gave up quite early, so we replaced it with a standard AC motor:
http://www.anderswallin.net/2005/11/testing-vfd-and-ac-induction-motor/
http://www.anderswallin.net/2005/11/motor-mount-for-new-opti-motor/

Then we thought the stock spindle and spindle bearings weren't that great either. So we got an MK3 spindle from littlemachineshop and built some bearing holders and a spindle box around that:
http://www.anderswallin.net/2006/10/a-new-spindle-for-our-opti-cnc-mill/
http://www.anderswallin.net/2006/12/new-spindle-installed/
It's belt driven with 1:1 ratio. Much quieter than the stock spindle.

Finally, the X-axis travel was a bit short, so we made a new table, and while at it replaced the dovetail ways with linear ways and the trapezoidal leadscrews with ballscrews:
http://www.anderswallin.net/2007/02/x-axis-progress/
http://www.anderswallin.net/2007/04/opti-bf20-on-rails/


hopefully we can show some videos with the DC servos soon. Maximum rapids should be much better than with the current steppers.

Whow! Hobby use?
Nice!

Yes, for hobby use. This mill has been used a lot to make plugs, moulds and rig parts for IOM RC yachts.

I'm also interested to see how good performance it is possible to get out of small mill like this with "little tuning".

Dudes, perkele!!!
That's a freakin good looking machine. Oh lucky I am, having a VFD waiting to be mounted. :)

Here's few pictures about column and base machining.

I had a chance to use VMC and machine the new T- slot table, drill and tap IKO rails M3 and ballscrews bearing housings M8 attachment threads to column and base at school where I did my CNC machinist vocational examination.

When we disassembled column from base, there came a big surprise: at factory they had "trimmed" column attachment
place with angle grinder! I machined that straight at school.

Column and base were first attached dovetail ways downwards against parallels, and attachment surfaces for
drilling and tapping operation were facemilled.

I could use the VMC only four days for this project, so it was not possible to do all parts needed to get the new table and IKO rails in use. After I had drilled and tapped the column and base, I took them back to my workshop and assembled Opti to original configuration. Then I machined ballscrews bearing housings, XY axis saddle plates etc. during weekends.

Next tuning part for the mill was new spindle:

MT3 spindle itself is from littlemachineshop:
http://www.littlemachineshop.com/products/product_view.php?ProductID=2027&category=

25 mm aluminium plates holding the bearings are machined with opti. I would have wanted to make those from steel as well as ballscrews bearing housings, but that was just too tough steel milling project for Opti at original configuration. It would have been possible with small cutters like 6 mm end mill, but it would have take so long time that I decided to use aluminium and bigger cutters.

There is 1:1 AT5 Belt drive. Bearings are FAG standard accuracy
angular contact bearings. Spindle radial runout is around 0.015 mm.

Yesterday 0.75 kW spindle motor was replaced with 1,5 kW motor.
It's the biggest motor that will fit in this spindle housing. Omron Varispeed V7 Vector VFD was also purchased about a week ago. With VFD we have used RPM' s up to 5000. Three-phase induction motor torgue start's to drop pretty
much after 3000 rpm/ 50 Hz, but at 5000 rpm there's still enough torgue to do light finish milling or drilling with small drills.

First tests showed that there's pretty much increase in torque and power with 1,5 kW motor:

I can now take 1,5 mm deep cut in aluminium with 40 mm face mill (40 mm wide cut) and it goes very well with 1200 mm/ min feed. RPM was 3000. That cut take's about 55% spindle power. 2 mm deep cut goes somehow with 900 mm/ min feed, but it doesn' t sound good anymore and machine doesn' t like it.

I would be interested to know how big cuts and what kind of feedrates it is possible to use in aluminium with with bigger mills like Grizzly G0519,
OPTI F 45 or Enco SQ COL MILL/DRILL???

JMI80, are you A. Wallin at the EMC mailing list?
Hmm... I just checked your website, yes you are Mr. Wallin. :)

JMI80, are you A. Wallin at the EMC mailing list?
Hmm... I just checked your website, yes you are Mr. Wallin. :)

that would be me...

so now the question is who are you really? 'Lernaean Hydra", "anonimasu", "jymm" ? :cheers:

Wow - that is a great 'conversion', or should I say rebuild!

I am realy envyous of your enclosure though - it's lovely :)

Is that cutting video with your 0.75kw or 1.5kw motor - you can really hear it bogging down as the cut begins, but it sounds completely chatter free to me :)

that would be me...

so now the question is who are you really? 'Lernaean Hydra", "anonimasu", "jymm" ? :cheers:

Nope, just Sven. But it was a looong time since I posted. I'm mostly reading.

I can now take 1,5 mm deep cut in aluminium with 40 mm face mill (40 mm wide cut) and it goes very well with 1200 mm/ min feed. RPM was 3000.

That's an extremely impressive removal rate for a machine of that size, in my opinion. Machine sounds very comfortable in the video, too. Nice work! There is no way my X2 would do that without a huge amount of chatter, if at all.

Wow - that is a great 'conversion', or should I say rebuild!

I am realy envyous of your enclosure though - it's lovely :)

Is that cutting video with your 0.75kw or 1.5kw motor - you can really hear it bogging down as the cut begins, but it sounds completely chatter free to me :)

Hi,

I can strongly recommend to everyone to do the enclosure if you are going
to CNC convert a mill or lathe! About five years ago we had absolutely
no idea how much chips and coolant there will be splashing around
and we learned it through the hard way...Efficient coolant system is
also a must.

That cutting video was shoot with 0.75 kW motor.
Motor almost stall when cut begins and lower feed rate
would have been good idea when cutter goes into material,
but idea of that video was to show what it sounds and looks like
when small mill and 0,75 kW motor is pushed to the limit!
Yes, that cut is chatter free.

I have now shoot few videos more with 1,5 kW motor.
I will have to transfer those to computer and upload to You Tube or to Google video, and I will post link here when those are ready to watch.

Hi all,

I shot few videos while machining those parts at the pictures below.

First phase roughing video link is:

http://www.youtube.com/watch?v=nibzhPfOF1Q

This video was shot after new 1,5 kW spindle motor
was installed. Face mill feed rate is 1200 mm/ min
and deph of cut is 1 mm. Two last cuts with face mill
are 2,5 mm deep and feed is 700 mm/ min.

8 mm 4 flute roughing HSS end mill takes 5 mm deep
cuts, and programmed feed rate is 600 mm/ min.
I set steppers acceleration pretty low to improve
reliability. Machine is not now pushed so close
to it's spindle power limits as it was in that first
video at google video server. I didn't want
take risk of steppers to lose steps when I'm shooting videos.

First phase finish operations are at:
http://www.youtube.com/watch?v=LzVZhDPXQ9k

Second phase drilling operations are at:
http://www.youtube.com/watch?v=pY7C_QDGNng
There is 5000 RPM and 600 mm/min feed.
Second and third phase videos were shot
when 0,75 kW spindle motor was in use.

And finally third phase videos:
http://www.youtube.com/watch?v=_d0uop0SFJ0

Parts attachment at this phase is not very sturdy,
so it's good idea to use little lower feed rates
with face mill. It would have been possible to
make jig/ fixture for the parts and get better
attachment for face milling, but it seemed
to work out like this so I decided to not
bother to make a fixture.

5 mm end mill makes 5,8 mm hole
for the reamer since that needed to be flat bottom hole.
5.99 mm reamer makes H7 tolerance hole for small
6 mm stainless steel bearing.

I only just saw this post - nice videos and great looking parts. What are they though - they look a bit like individual turbine blades?

I only just saw this post - nice videos and great looking parts. What are they though - they look a bit like individual turbine blades?

Hi,

Those are IOM RC yacht ball-raced gooseneck bearing housing parts.

Prototype 2 looked like this:
http://www.anderswallin.net/2007/05/gooseneck-prototype-2/

And this third version idea was to make parts which will
fit to different mast diameter's from 10.9 to 12.7 mm.

Great Machine!

Top Notch.

I am quickly learning your advise about the requirements of good enclosure.

Hi everyone,

some serious re-building of the machine has just happened and we have installed DC Servo motors which are direct coupled to the 2.5mm/rev ballscrews. There are a couple of blog posts and a couple of videos out there for you guys to look at:

first test with servo-driven X-axis:
http://www.anderswallin.net/2008/04/x-axis-test/

first cut with a 40mm face mill:
http://www.anderswallin.net/2008/04/first-cut-with-servo-mill/

first serious job, a steel keel bulb for a model yacht:
http://www.anderswallin.net/2008/05/bulbs-of-steel/

more steel milling videos:
http://www.anderswallin.net/2008/05/bulb-milling-videos/

The machine also now has a home-built jog-pendant:
http://www.anderswallin.net/2006/11/jogging-emc2/

Next we hope to install a spindle encoder which will enable rigid tapping. Any questions on the EMC2 / m5i20 control electronics or on the mechanics of the machine just ask and I will try to answer.

Next we'd like to build a lathe from scratch but I'm not sure when we'll have time for that...

have fun,

Anders

I should add that the rapid feedrate is now set to 5000 mm/min. That's around 197 IPM for those of you who like to divide everything by 25.4

Thanks for the update - it really is great to see some more of this amazing conversion/rebuild in action. Keep up the great work!

you are the first i see that doesnt use the 4 or 5mm ballscrew pitch.
i wanted to go for 2mm pitch myself on my x3 in the future.
do you have good results with your 2.5mm ballscrew?

We wanted to directly couple the DC servos to the ballscrew, so we thought it wise to select a small pitch screw to get enough torque and force. That also gives good resolution with the 1000 ppr (4000 edges per rev) encoder. The downside is slower rapids - the theoretical maximum with 3000rpm servos is now 7500mm per min, and in practice we get about 5000mm per min. This is more than enough for a hobby machine.

Congrats for very successfull rebuild! Clean sound without resonance. Clearly not a toy :)

This is freaking awesome stuff right here! Awesome!


-Jason

Hi,

I uploaded a new video "Making a fixture for drilling operation"
at http://www.youtube.com/JMI80

There's pretty fast aluminium roughing (feedrate 2000 mmm/ min) with 8 mm end mill shown. NC program was not perfect and machine allmost stops when there comes tight radius and lot's of Gcode, but since that was one off part it's not so critical.

There's more information and pictures about these parts at my friend website at http://www.anderswallin.net/2008/05/finderscope-rings/

Regards,
JMI

After mounting a 500 cpr encoder on the spindle motor we now also have rigid tapping:

some M3 threads:
http://www.youtube.com/watch?v=9hrduckmcd4

and some M6 threads:
http://www.youtube.com/watch?v=uhaKQH2CCGI

AW

Nice stuff!


-Jason

After mounting a 500 cpr encoder on the spindle motor we now also have rigid tapping:

some M3 threads:
http://www.youtube.com/watch?v=9hrduckmcd4

and some M6 threads:
http://www.youtube.com/watch?v=uhaKQH2CCGI

AW

Wow, this machine just gets more and more impressive! When's your tool-changer coming? ;)

So how does rigid tapping work in EMC? Do you still have a 1.5kW induction motor and VFD on the spindle? Does EMC just command a spindle stop at the bottom of the stroke, and then slow the Z-movement as the spindle spins down, and then accelerate back up out of the hole as the spindle spins back up in reverse? Is EMC really turning a dumb VFD + and encoder into an AC servo? It's very impressive however it works!

Yes we demand that you add a tool changer! Very impressive!

So how does rigid tapping work in EMC? Do you still have a 1.5kW induction motor and VFD on the spindle? Does EMC just command a spindle stop at the bottom of the stroke, and then slow the Z-movement as the spindle spins down, and then accelerate back up out of the hole as the spindle spins back up in reverse? Is EMC really turning a dumb VFD + and encoder into an AC servo? It's very impressive however it works!

As far as EMC2 is concerned, the spindle runs in open-loop. I command an RPM from EMC2 which is output as a pulse-train to the VFD and the VFD will spin the induction motor at this RPM (more or less). Internally the VFD uses back-EMF, measured phase current and such things for vector control, but these signals are not wired to EMC2.

The Z-axis is then 'slaved' or 'geared' to the spindle encoder. So instead of the set-point for the Z-axis PID coming from the trajectory controller this set-point now comes from the spindle-encoder (multiplied by some scaling and some offset added). There's a detailed description of the G33.1 code I used on the wiki
http://linuxcnc.org/docs/html/gcode_main.html#sec:G33,-G33.1:-Spindle-Synchronized

at least this is how I understand it right now...

I don't think the toolchanger is coming anytime soon :)

AW

I'd forgotten that induction motors were pretty much synchronous! That G33.1 is pretty sweet - the sooner I move to EMC, the better!

Hi all,

I made short IOM RC yachts tiller arm production
run at the weekend and shot video from that. Here's
also couple pics about the setup. There's now finally three vises in use on our mill.

You can find video from there:

www.youtube.com/JMI80 and it should also appear below.

YouTube - Machining of IOM yachts tiller arm's

For this video, all tools except 8 mm rougher are
run without coolant, so you can see much better what is happening. Didn't want to try what happens if I run that rougher without coolant since I programmed pretty aggressive feedrate for that..

NC spot drill makes couple stupid moves but I didn't bother to fix those anymore at late in the evening...

Awesome stuff. Look exactly like servo horns :) I'm into Helis and planes myself. Great stuff!


-Jason

Thanks for posting that - I love watching this machine run :)

Hey, I just wanna say I enjoy all of you who share your videos of builds and or upgrades to your machines! Man, they are awesome! it's the epitome of what homeshop machining means. I just can't figure out why hobby machining has never made it to TV...lol, then again I can probably host a cable access show....lol...with clips from youtube...lol, yeah, it could work, it could work, it could work...(If Dorothy can find herself home after repeating it three times, maybe we can get machining on TV...lol) Thanks guys for your videos on your projects, builds and test runs... keep the videos coming and the good work up...

-eddie, satisfied viewer.

Very impressive. I am still stuck in the 1 op mode. I have so much to learn about this.

How did you set up the Offsets for different vices? Were they creted as different gcode ops and then tied together using the offsets?

I just really don't know how that is done. :confused:

Very impressive. I am still stuck in the 1 op mode. I have so much to learn about this.

How did you set up the Offsets for different vices? Were they creted as different gcode ops and then tied together using the offsets?

I just really don't know how that is done. :confused:


Hi,

Sorry about late answer, it's been a while since I visited in CNC
Zone and for some reason I did not get any email from cnczone
that there has come reply to this post. But let's go to your
question:

Using offsets for different vises is pretty simple. Maybe simple
example program is best to explain their use. Let's assume
that you have three vises, there's one part in each vice and you
want to do NC spot drill operation for all parts. Let's also
assume that part zero is at part's left upper corner, and NC spot
drill hole place will be X10.0 Y-10.0 from part zero

%
O1234
G90 G80 G40 G49
G91 G28 Z0.0
G91 G28 X0.0 Y0.0
G90 G10 L2 P1 X50.0 Y-100.0 Z-300.0
G90 G10 L2 P2 X200.0 Y-100.0 Z-300.0
G90 G10 L2 P3 X350.0 Y-100.0 Z-300.0
T1 M6 (NC SPOT DRILL)
G54
G0 X10.0 Y-10.0
S6000 M3
G43 H1 Z5.0 M8
G81 G98 X10.0 Y-10.0 Z-2.0 F600.0 R5.0
G55 X10.0 Y-10.0
G56 X10.0 Y-10.0
G80
G0 Z50.0
M5
M9
G91 G28 X0.0 Y0.0 Z0.0
G90 G80 G40 G49
M30
%

That should do the NC spot drilling job( if I can still do manual
programming...). At the beginning of the
program there are G90 G10 L2 P1 XYZ lines. In those you put
the distances from machine zero(reference point) to part's zero
points. P1 is for G54, P2 is for G55 etc.

I learned to use G90 G10 L2 P1 XYZ at work with Fanuc
controls. It also works with EMC2. I don't know what control
you are using, but maybe G10 will also work with Mach3 or
similar.There should be something about G10 in manual if it can
be used.

Those IOM yachts tiller arm parts were programmed with CAM.
I made separate programs for each vice and I combine those into
one manually. That kind of programming is used regularly in
commercial series production machine shops. It's also good
programming exercise for home shop machinist!

Thanks, that helped out a lot. :)

I do use Mach3, so I will try and use that when I can.