My DIY-carve

you are killing me with your clean wiring :wink:

Minor update, but no images to show yet.

Soldered up the signal wires for all axes and briefly tested the X and Z axes.
At the moment running full step (1/1 stepping) after performing an autotune. Compared to the TB6560 drivers I use at the moment it is very quiet as 1/1step with those is quite harsh sounding.

With the TB6560ā€™s and 24V PSU my max real-life RPM limit is about 500 which equates to about 2500mm/min for rapids. (5mm travel per turn)
With a 48V PSU (dialed down to 45V) I should expect an ~80% increase in rapids, but the main benefit is the usefull torque curve is pushed higher at higher feeds.

See image below:
SMBFig2

With the TB6560ā€™s I have 2500mm/min for rapids and 500-1000mm/sec*2 at 24V.
With the DM556ā€™s I easily got 4000mm/min but have not dialed it in further. Did not play with acceleration rates as I simply ran out of time.

Regarding speed I have one limiting factor which differ from Xcarve which is full step resolution (travel)
I will use SFU1605 screws an all axes, and sport 5mm travel per turn => 5mm / 200step = 0.025mm
In effect it is geared down compared to the Xcarve, more torque, finer step resolution at the expence of all-out rapid speed

Since my travel is 5mm / turn and steppers have a typical max RPM somewhere around 1000-1200 my absolute possible max rapids is 5000-6000mm/min. The Xcarve have a much higher travel per motor step thus faster.

Anxiously waiting for the 4th driver to arriveā€¦ :slight_smile: Once it does the new controller is actually ready to be used, remaining all secondary bells and wisstles like buttons/relays and the estetics :smiley:

Quick update:

Still waiting for the 4th stepper driver but borrowed a DM542 while I am waiting, so I could get the bare controller up and running. Wired it all up yesterday and have now briefly tested that everything works - which it does :slight_smile:

Base parameters at this time which seem to work is:
$110=4500mm/min
$111-112=5000mm/min
$120-122=500mm/s^2
Drivers are set to 3A RMS
Running 1/2step on all axes (400step per revolution, theoretical resolution per step = 0.0125mm or about half a thou inch)

Aside from the speed the sound is much smoother than the TB6560Ā“s, despite running coarser step. The DMĀ“s have only been hooked up and done a quick autotune sequence before I started playing with the speed/acceleration.

Excited :smiley:

I now have two complete controllers:
Old 24V and TB6560-based
New, 45V and DM556/DM542 based (PSU dialled down from 48 to 45V)
Time willing I may make a comparison video.

2 Likes

Canā€™t wait to see what this thing is capable of. Great job!

Thanks @StuartPearson, so am I :smiley:

Now much progress visually as I have been in the process of wiring the control buttons etc, its the small stuff that takes time!
At the moment the controller is operational, with homing switches and Pause/Resume/Abort buttons complete.
Also spent some time debugging as my Z would suddenly only move up, did eventually find my loose wire :slight_smile:

I have decided that my relays will be outside the controller and placed in a separate housing the the AC outlets. This mean I will need to make a quick-connect signal wire between the controller and relay box, this also add better flexibility as far as placement goes. Separating AC from DC is also a benefit.

An observation:
My X rapid is less than the other two axes, it is on X I am using the loaner driver (DM542) which is different than the others (DM556) Both Y & Z will hit 5000mm/min rapids but X will not, hopefully I can get a bump-up when my 4th DM556 arrives.

1 Like

The first two test carves with the new controller is done, main objective was to test/verify that all is in good working order.

HDU plastic sheet carved at 4000mm/min for X/Y/Z - no problem, it ripped with a 3F bit. Full WoC (3mm) and 3mm DoC at 8-17k RPM

Aluminium stock, 4mm 2F bit used.
Here is chip thickness the key parameter which suggest 850mm/min for feed at 17k rpm. Tested down to 6mm DoC and 1mm WoC => 5.1cm^3/min in MRR.
This isnt a test that highlight the capacity of the new controller, but overhead is always welcome :slight_smile:

For fun I tried to hold back the X-axis during rapid transitions (4000mm/min for X) by hand, I was completely unable to provoce it to stall :slight_smile:

2 Likes

Would love to see some footage :slight_smile:

@StuartPearson and others who are interested.

This was the very first carve done to test cutting strategy and what I was achieving in dimensional accuracy.
Before rebuilding the controller I couldnā€™t go past 2500mm/min (rapids) consistently, this time 4000mm/min appeared to be a breeze.

Cutting parameters:
Fusion360 2D Adaptiver Clearing strategy used
17k RPM
4000mm/min feed rate
DoC 8mm
WoC 0.1mm
Chipload 0,11mm
Chip thickness 0.037mm
MRR a modest 3.2ccm/min

Here you go, 1st half :

2nd half:

1 Like

nice!

Pushing the limits for my machine, and a ā€œchip restrainerā€ :slight_smile:
MMR=10,2ccm/min (initial path and 6,8ccm/min for the adaptive)
Can smell the heat of those big chips :slight_smile:

7022 aluminium used.

4 Likes

Another video showing my current project in the making, a miniature turbine for RC jets :wink:

I had to spend some time getting my machine fine-tuned as the tolerances are slimā€¦
Also had some sudden connection issues that caused me some grief.

1360mm/min @ 17k
6mm 2F going 3mm deep per pass / 2,4mm stepover
Two parts are shown here, the diffusor and its cover plate.

2 Likes

Wow, look at all those flying chips! Would be neat to see the end result. Thanks for sharing.

1 Like

Howā€™s the painterā€™s tape & superglue recipe holding on mdf? Itā€™s been on my list for a while but still havenā€™t tested it.

@EliasPolitis - my waste board is not MDF, it is water resistant particle board intended for wet room flooring.
I suspect MDF that have been skim cut dont hold tape that well.

The surface area for this particular carve is roughly 30-35sq.cm and hold just fine with <10ccm/min. Alu stock is nominally 15,5mm thick btw. I really need to forcefully pry it off before it start to lift, its solid. I only use additional hold downs after parts have been cut through.

Haldor, read through your post again because Iā€™m looking for some decent starting place with aluminum. Just finished doing some rigidity improvements and I picked up a bunch of plate aluminum and a destiny tool viper 1/4" two flute bit. I need to find out some good feed rates. Iā€™ve also added a mister with denatured alcohol much like yourself. Iā€™m curious if you had any tips you learned that might help me. Also, did you have any two flute 1/4" end mill speeds/doc numbers you should give me to start with?

Destinyā€™s specs have me confused. They listed an IPT chip load of .004-.005 for their 1/4" end mills, which is great.

The confusing part is they also list a minimum SFM of 1200, which causes all kinds of problems. Using just the chip load I could run reasonable feed rates for my machine, ex. 8600rpm x 2flutes x 0.004IPT = 68.8ipm. However, if I append to the minimum SFM of 1200, that means I need to run at 147IPM, which is crazy fast. I believe my machine could do it, but the margin for error is so slim Iā€™m not too eager to try. Is my math right?

SFM is the rotational speed of the cutter, tip velocity, not feed rate :slight_smile:
Learned the hard way :rofl:

The formula for cutter velocity for RPM is (in metric, 1200 feet / min = about 365m/min):
[RPM] = (SFM[m/min] * 1000) / (3.14 * CutterDiam [mm])
So 365m/min*1000 / (3.14 * 6.35) = RPM =18.350

So dial in your router for approx 18k RPM.
Then follow the chip load calculus Destiny provided :slight_smile:

I use 6mm 2F a bit and the cut parameters for me is:
RPM 17k
Feed rate 1360mm/min (680mm/min per tooth)
Machine rigidity will determine how deep per pass, start shallow and increase this value once confidence is growing.
Try 0.02" DoC to start with

The bit specs that follow my 6mm bits suggest Vc=500m/min and chip load 0.05mm/tooth which is less than Destiny.

Hope that helps :slight_smile:

I thought I understood the SFM part, I was just surprised Viper listed the minimum for the Viper tools as 1200. Because itā€™s 1200 I thought that meant I have to run 18k rpm and 147ipm (!) which is what concerns me. Thatā€™s quicker than I run through any other material.

I see youā€™re talking about 1360mm/min, which equates to 53IPM, which is way lower than what I was coming out with. I must be missing something. Doesnā€™t that fall below their 1200SFM minimum?

Here is what I calculated, tell me if I made a mistake here, because this is saying I need to be running at 147ipm (3,733mm/min)

Iā€™ve went through Destiny Toolā€™s info sheet and calculation sheet on SFM and I keep coming back to 147ipm is their recommended speed, and itā€™s all do to the 1200 SFM minimum they specify. It would seem a lot of people either ignore this minimum, or itā€™s not necessary. They say in their FAQ that SFM should be as high as possible to maximum production speeds, but that seems counter intuitive to also place a minimum on it. Thatā€™s whatā€™s making my question if people are just ignoring their minimum SFM of 1200.

@Pyrex

This is the spec sheet that follow my primary tools:

Destiny suggest a chip load that is basically 2x what Sorotec suggest for mine which pushes the feed rate up there.
The spec also assume a rigid, non-hobby CNC so we need to devaluate based on that.
Chip load also must involve tool flex/deflection/runout as this add to the chip load aswell.

With smaller diameter tools the RPM needed to match SFM exceed router RPM capacity so we just fudge it by going as fast as we can/dare and adjust feed rate (maintaining chip load) accordingly.
The target SFM number is the cutter speed optimum slicing speed where the material ā€œsliceā€ the best with optimum heat distribution etc.

Per Viper mill&feed calculus the 147ipm seems legit, tho may not be transferable to the Xcarve.

I do however think that the tool path strategy is key here
If you go on the outside from stock and cut inwards, taking off 0.04" per pass may work.

Like this where I am cutting at 4000mm/min with a 6mm tool, WoC=0.1mm (DoC=8mm)

The same feed rate would not work for a pocket cut where WoC is much larger, like this:

(stepover is 0.04mm)

okay thatā€™s exactly what I figured. Both Niagara and Gorilla both listed chip loads of .002, and I could not understand why Destiny was listing .004, which made all of the feed calculations seem bananas. Also, most of these manufacturers list a minimum SFM of 800, not 1200.

Taking this one step further, the feed rate * DoC * WoC = MRR and this is ultimately the threshold for any given CNC.

Fr * WoC * DoC = MRR, cubic cm per minute
4000mm * 0.1mm * 8mm = 3,2ccm/minute
1360mm * 2.4mm * 1mm = 3,2ccm/minute

With my setup I can push:
1360mm * 6mm * 2mm = 8.1ccm/minute (tested)

My rapids are 4000mm/min and torque at speed is low so I can not push my MRR up at this feed rate.