Milling Aluminum Long Board truck

Post Reply
MarkVa1
Posts: 190
Joined: Mon Aug 04, 2014 12:56 pm

Milling Aluminum Long Board truck

Post by MarkVa1 »

Looking for opinions / thoughts for milling some long board trucks for an electric skateboard. Trying to use the experience to get my teenage son into machining and such.

I have yet to do any aluminum milling with my KRMX02, but have watched the videos on the the Kronos website. Looks like 2 flute carbon end mills can do the trick. I'll need to make some type of jig to hold / rotate the piece for the various angles. Plan to mill the motor mounts and maybe even the 36 teeth pulleys. I think 6061 aluminum should be strong enough.

Just wondering if anyone has done something similar with their KRMX02 and can share some pointers.

Thanks,

Mark.
baysale976
Posts: 494
Joined: Mon Dec 31, 2012 11:07 am

Re: Milling Aluminum Long Board truck

Post by baysale976 »

I don't have much to share, except about work holding: There is a lot more force than you think.
Make sure it is held very solidly.
msimpson
Site Admin
Posts: 3176
Joined: Tue Mar 30, 2004 6:19 pm

Re: Milling Aluminum Long Board truck

Post by msimpson »

Yep, it all starts with holding your stock as secure as possible. If thats not good, nothing else matters.

I see a machinists vice in your future.
MarkVa1
Posts: 190
Joined: Mon Aug 04, 2014 12:56 pm

Re: Milling Aluminum Long Board truck

Post by MarkVa1 »

:D I was thinking about that! I’m surprised how low $ the aluminum flat bar costs. I will probably buy some larger pieces and use some symmetrical holes to secure it to the table and allow for milling both sides ... probably going to be large learning curve on this one :D
msimpson
Site Admin
Posts: 3176
Joined: Tue Mar 30, 2004 6:19 pm

Re: Milling Aluminum Long Board truck

Post by msimpson »

I would recommend looking at all my working with aluminum videos and web pages.

Here some information on the vises that I use. Not real expensive.

viewtopic.php?f=41&t=2040&p=10504

I have two of the 2" machinists vises and they handle pretty much most of my aluminum chores.
MarkVa1
Posts: 190
Joined: Mon Aug 04, 2014 12:56 pm

Re: Milling Aluminum Long Board truck

Post by MarkVa1 »

Thanks Michael - surprisingly inexpensive. I read a little about the use / importance of parallels so I ordered the one with the parallels. Should hold everything I need as a 3" piece is my widest stock. Looked into the Kurt vises but a little pricey for what I need.

Design is almost done. Waiting on the bushings to arrive as getting true dimensions is hard online, and I need my pivot to precisely fit...

I'd like to mill the pulleys myself but the tooth spacing is a radius is 10mm deep and the radius is less than any bit I have that can cut that deep. Only way I've seen it done is sideways on a lathe with a flywheel tool. And I don't have a lathe... Otherwise I think I can make the trucks, brackets and braces...

Mark.
Attachments
Screen-Shot-12-17-20-at-04.jpg
Screen-Shot-12-17-20-at-04.56-PM.jpg
baysale976
Posts: 494
Joined: Mon Dec 31, 2012 11:07 am

Re: Milling Aluminum Long Board truck

Post by baysale976 »

Our HS Robotics team makes these pulleys by drilling (with the CNC) the correct diameter holes first, then machining at the right diameter to expose the needed tooth pattern. They tried doing it after cutting out the diameter, but the drill was not rigid enough to drill half a hole.
msimpson
Site Admin
Posts: 3176
Joined: Tue Mar 30, 2004 6:19 pm

Re: Milling Aluminum Long Board truck

Post by msimpson »

If you are not going too deep, I have found using an end-mill smaller than the diameter and milling them using ramps. Do them about .003 shy of the diameter. Then do a single full pass at proper diameter.

Add this method and a harmonic drive and some sort of collet holding system and you could make all kinds of gears very accurately.
MarkVa1
Posts: 190
Joined: Mon Aug 04, 2014 12:56 pm

Re: Milling Aluminum Long Board truck

Post by MarkVa1 »

From what I've researched, a 40 Tooth pulley is about 64 to 65 mm in diameter. The resulting drill holes for the teeth are about 1.3 to 1.5mm in diameter. I'm looking to hold a 15 mm belt, so the depth might be 16 mm.

I'm not sure where to find that type of bit with such a small diameter but enough cutting depth to bore down 16 mm? Drilling the holes first makes sense. I'm not in a hurry so I can take the milling slow, but most of the bits I've seen this small have a very short cutting depth.

Thanks

Mark.
baysale976
Posts: 494
Joined: Mon Dec 31, 2012 11:07 am

Re: Milling Aluminum Long Board truck

Post by baysale976 »

Here is one example of such a drill bit. https://www.mcmaster.com/29355A19/ The difficulty will be getting a collet to hold it. I am not recommending this set, but it is but one example that contains a suitable collet for 1.5 mm drill bits. https://amzn.to/2M1UUVJ

An option is a carbide bit like https://www.precisebits.com/products/ca ... &filter=12, which has a 1/8" shaft, but only a 10 mm depth of cut.

Perhaps you could just mark the holes with a CNC (drill to 0.030 depth with an 1/8" bit) and complete them in the drill press. But you will need robust and repeatable workholding to ensure the pulley remains concentric.
MarkVa1
Posts: 190
Joined: Mon Aug 04, 2014 12:56 pm

Re: Milling Aluminum Long Board truck

Post by MarkVa1 »

baysale976 wrote: Tue Dec 22, 2020 2:22 pm Here is one example of such a drill bit. https://www.mcmaster.com/29355A19/ The difficulty will be getting a collet to hold it. I am not recommending this set, but it is but one example that contains a suitable collet for 1.5 mm drill bits. https://amzn.to/2M1UUVJ

An option is a carbide bit like https://www.precisebits.com/products/ca ... &filter=12, which has a 1/8" shaft, but only a 10 mm depth of cut.

Perhaps you could just mark the holes with a CNC (drill to 0.030 depth with an 1/8" bit) and complete them in the drill press. But you will need robust and repeatable workholding to ensure the pulley remains concentric.
Thanks - now all the discussions I've read about precision collets makes sense... :)

I may give the McMaster Carr bit (or something similar) and precision collet a try. Worse case scenario - it doesn't work and I buy the pulleys... but trying to use my KRMX02 to do it is the fun part!
MarkVa1
Posts: 190
Joined: Mon Aug 04, 2014 12:56 pm

Re: Milling Aluminum Long Board truck

Post by MarkVa1 »

"The difficulty will be getting a collet bit to hold it..."

I ordered some ER20 collets for my Bosch 1617 but they don't fit. I thought I read online that the 1617 uses ER20 collets. After it didn't fit, I searched some more and read that no US router products use ER Collets? If I go the Precise Bits route, they are specifically made for the router and not actually ER20 standard sizes...

It's all a bit confusing and annoying... everyone doing the same thing slightly differently is ridiculous :D

Is Precise Bits the only way to go for smaller collet sizes on a Bosch 1617? They are Imperial and not metric... I was planning to mill with some 2mm and 3mm end mills, but at this point I'm not sure how to find a collet chuck nut to hold the right collets.... :shock:
baysale976
Posts: 494
Joined: Mon Dec 31, 2012 11:07 am

Re: Milling Aluminum Long Board truck

Post by baysale976 »

MarkVa1 wrote: Wed Jan 13, 2021 5:39 pm everyone doing the same thing slightly differently is ridiculous
Yep, kinda like different cars using different lug bolt patterns. Everyone thinks they have the best solution.

Ideas:
1. Google "collet for bosch 1617 router" and check out the results. Elaire Corp has a good selection. They say they are R24.
2. Someone on YouTube converted their EVS1617 to ER20. It is under 7 minutes long, watch it.
3. It is possible to make your own collets. You do need a horizontal mill and metal lathe and considerable skill, but it is not impossible. Then the center hole can be any size you like, to hold anything.
(In the machining industry, a 'blank collet' is something you keep in stock, to bore it out to hold some odd size workpiece or tool. They are not expensive and, most importantly, not hardened so they can be machined. But the Bosch is not a 'standard' collet (like ER20) so you'll never find a blank collet AFAIK.)

As I wrote, the collet to hold the tool is the hardest part.
MarkVa1
Posts: 190
Joined: Mon Aug 04, 2014 12:56 pm

Re: Milling Aluminum Long Board truck

Post by MarkVa1 »

Got the board done! Finally. The electrical and speed control items were a big learning curve for me compared to the CNC work. The drop down looks cool but isn't providing enough clearance so I'm milling new aluminum extensions today to rise up instead of drop down. But the motorcycle helmet is on it's way and my son will hopefully be able to ride this through college which will be 8 years of use... At least that is the goal! If he doesn't ride it I will!

Thanks to everyone on here for CNC recommendations / settings advice. Helped a lot!
Attachments
IMG_0368-1000.jpg
IMG_0369-1000.jpg
baysale976
Posts: 494
Joined: Mon Dec 31, 2012 11:07 am

Re: Milling Aluminum Long Board truck

Post by baysale976 »

Very nice!

Care to share your choices of tooling, feeds & speeds, and cooling/chip management with us?
We're all about learning new things, and you have some experience now that I, for one, would love to hear.
MarkVa1
Posts: 190
Joined: Mon Aug 04, 2014 12:56 pm

Re: Milling Aluminum Long Board truck

Post by MarkVa1 »

Sure! I guess I have done enough where I can add some potentially helpful tips :-)

For aluminum, my limiting factor is certainly the Bosch 1617 EVS router I'm using. It's been great for what it can do and runs like a champ, but it cannot mill aluminum in the recommended ways per many YouTube videos. It doesn't have the rigidity to do 3D Adaptive clearing by coming in from the side of the piece and controlling the optimal load which the more advanced spindles seem to perform with ease. I often see online depth of cuts in the 1/4" to 1/2" depth range but controlling the optimal load - no way with this router. Accordingly, I just decided to go shallow and accept the long milling times per piece. I run it at it's top speed setting of 6.

I'm referencing Fusion 360 CAM. As a starting point, I use 0.02" DOC, 50 IPM, and an optimal load or stepover resulting in 1/2 the bit diameter cutting. I have used 1/2" bits, but I now try to keep my max bit size at 0.25". If it's roughing I'll set it to "both ways" and for finish cuts its a climb cut or "left". Adaptive clearing is important as trying to 2D contour results in too much of a load and goes bad quickly. Lack of chip evacuation and the bit getting gummed up happens fast! So I'm often milling the entire aluminum stock except for what is remaining for the finished piece. I don't cut anything out of aluminum like you can with wood. Which makes using dowels and such to rotate pieces for two sided milling a challenge. So I milled a fixture plate with dowel holes and such to secure wood / 3D printed jigs to help accurately locate and flip pieces. Also posted elsewhere on here about setting up the depth probe to locate the X and Y 0,0 as well which has been helpful with aluminum.

I'll typically face the rough aluminum to final depth and use a micrometer to check. I'll clamp in my milling vice or use the painters tape / CA glue trick to secure. The CA glue trick is a Godsend! If I tape and glue, I'll run the facing operation on the waste board first to ensure a flat surface. So in Fusion, I typically copy / paste the same part a few times and copy / paste the set up. Reason being, my first set up is with the stock at initial depth, second set up is after facing it to final depth. I try to chamfer any and all edges. If you run 3D adaptive with the chamfers on the model it will try and mill the chamfers. You can use the 2D Chamfer on the model hard edges but that only works on 2D. I'm often chamfering 3D edges, so I use a 0.25" bull nose bit and 3D Scallop routine to accomplish that. There is a Fusion 360 tutorial on how to do that online somewhere. The settings are not obvious but it works. So that's a reason for multiple copies of the same model. Sometimes I'll add patches to ensure the Adaptive and Parallel routines don't deal with the holes / etc.

I may increase the depth of cut to 0.025" but never above 0.03" - so no mater what I'm doing it can take several hours to mill one side of a piece. The logic is this will dull the bits sooner, so I use cheaper SpeTool bits from Amazon. I think a pack of 5 bits at 0.25" two flute is $40. They work well for this application. Haven't had a dulling issue yet. But when that happens they are cheap to replace.

In general, I try to make the 3D adaptive work with a 0.025" maximum roughing step down and an optimal load of 0.1. This essentially uses about half of the bit diameter (0.25" bit for example) and takes a very shallow pass. I use a feed rate of 50-60 IPM. I'll leave 0.005" of material on the Radial Stock for a climb cut finish pass - typically a 2D contour with a step down of 0.5 inches. I try not to use Pocket Clearing as it engages to bit too much early on - there's a lot of discussion online about Adaptive vs Pocket.

For smaller holes, I'll use a 1/8" end mill. If you read about aluminum milling a single flute is recommended but they can be harder to find / more expensive so I pretty much have 2 flute flat endmills. As an example, for my 1/4"-28 holes I'll use a 15 IPM speed on a 2D contour, but I'll set the "ramp" to ensure it takes less than 0.01" per revolution. Essentially ramping all the way down through the hole. Maybe even more like 0.005" per revolution. It's slow but effective. Compressed air for chip removal is a must. I don't have any attachments so I just keep my air compressor handy and blow air on it about twice per turn. Metal chips go everywhere as I am not using an enclosure, so it's just some vacuuming time when I'm all done. No big deal. I don't trust my enclosure vacuum set up to effectively remove chips from small / deep holes and aluminum can gum up and go real bad really quickly with the wrong settings / conditions.

For larger holes / maybe a 0.25" bit at 30 IPM. Again, adjust the ramp angle to keep the amount of material removed per revolution to 0.008" or something close to that. I just eyeball it now on the Fusion preview. If cutting the exterior of the hole leaves material in the center, I'll often sketch a smaller circle and use the sketched object to first remove the inner material then finish with the actual hole contour. I just find ramping a 2D Contour an easy and surefire way to mill holes in aluminum. If I have to run two routines per hole that's fine with me.

For all holes I'll leave 0.005" material and clean that up with a finish pass climb cut. I'll typically make the rough cuts climb cut as well for the holes.

So it's slow, but so much better than me trying to accurately use a drill press and such :D I'm on a tapping spree, so I try to ensure the tap hole is deep enough for 6 threads from the screw. I've read any more than 6 threads engaged doesn't increase the holding strength. Loctite and threaded holes in aluminum seem to be plenty strong for my purposes. Inserting McMaster-Carr parts helps with this evaluation.

I'm not using any lubricant - so all dry cuts. I want those chips out and away from the cutting area. I'll run a finish pass with a Parallel routine using a 0.25" bull nose bit at a stepover of 0.0125" - this takes a while to complete, but results in a nice pattern and I don't need to sand or do other finish work. I'm not a patient enough man to enjoy sanding and finishing aluminum. So I let the machine do it. The finish from dry milling / facing is OK, but nowhere near as nice as a professional job with lubricant. So the parallel with the BN bit is a good second place alternative for me.

Chamfers - typically 25 - 30 IPM and a Chamfer width and Tip Offset of 0.02" each. Fusion defaults to 0.04 but I think that's too big for my purposes. This is with a 90 degree V bit. That's for the 2D Chamfer CAM routine. Anything in 3D needs to use the Scallop trick mentioned above.

Tolerances - space between my object walls and the jig walls as an example - typically 0.5 mm. Don't ask me why I switch to metric, I just seem to have an easier time remembering 0.5 mm for spacing. :D But since everything online I looked into is Imperial for CAM I stick with that.

For smaller bits - I bought some end mills from Kodiak Cutting Tools. I've gotten as small as 0.078" diameter. They had a close out sale on 4 flute micro endmills which is about 3 flutes too many, but with keeping such shallow cuts it doesn't have a negative impact. Same slow speeds / small incremental depths on the ramps, and lots of compressed air. Bit I'm able to cut some nice small holes and such.

Lastly - sound! Milling aluminum is very noisy and its obvious when something is wrong! It will sound awful and you'll need to hit the kill stich quickly and turn off the router quickly. I may not hover over the machine, but I'm always within ear shot of it as best I can. Since parts take a lot of time per my methods, I always try to have something else to do while the machine is milling.
baysale976
Posts: 494
Joined: Mon Dec 31, 2012 11:07 am

Re: Milling Aluminum Long Board truck

Post by baysale976 »

Thank you! Very detailed and helpful.
Post Reply

Return to “General CNC”