[ChrisAttebery]

I try to fixture up all of my production parts if I know they will sell enough to make it worthwhile.

Before I had my CNC mill I had an Enco mill/drill. Around 2011 Losi released the SCTE 1/10th scale 4wd RC truck. It was awesome, except for the fact that the cross pins in the differentials were butter soft. They would be worn out in 10 runs or less. I found a prehardened 3mm dowel pin that would fit, but it needed a 3mm x 1.5mm groove cut across each pin. I cut 3500 pins in a fixture one at a time that year. It took Losi 6 months to get their production worked out. I had factory drivers calling me for pins. After I built my CNC I made this fixture to cut 50 at a time:




I also sold a battery tray for that truck that moved the battery back about 1". I made this fixture to hold 10 trays at a time. Ignore the missing Y cover. This is right in the middle of CNC upgrade fever:






This fixture was for a chassis plate for a Kyosho 2wd RC car. The stock ones were pretty brittle. I made a couple hundred of them out of aluminum.






The parts I'm working on now are for high power rocketry and they sell in pretty low volumes. For these I set up soft jaws and cut 1 part at a time. It isn't worth fixturing up at the moment.

Attachment 303252

Attachment 303254


I'm not usually in a big rush so I set up conservative feeds and speeds and let the machine run. Sometimes it's more convenient to have a longer run time. Those chassis plates would run 1-2 hours between tool changes. I'd start a batch, go inside and have dinner, bath the kiddos, put them to bed and the machine would be ready for the next tool.

[dammachines]

I thought that bottom left part looked familiar... Maybe I'm spending a little too much time on the Fusion 360 forum.

Dave

[lcvette]

Hahaha... I saw that there too.... I played with fusion for a while yesterday and this evening, and have it pretty well figured out bit its kind of wonky feeling since I have become so accustomed to solidworks, I'm sure with time the workflow could be easier bit I prefer the feel of solidworks still I think.

And I definitely like Camworks better as a CAM option. It has ALOT more depth which was a steeper learning curve, But it also allows alot more flexibility then fusion 360. I also really have fallen in love with the build in feeds and speeds database for all the different materials and all the included tooling. They are pretty damn spot on even with my puny little G0704.

It's nice just setting the highest spindle speed and then adjusting the feed per tooth and stepover and everything else is calculated for you.. Super convenient.

One tool path I prefer in the fusion 360 cam though is the circle pocketing adaptive clearing, it seems to be faster. Although I haven't played with Camworks other roughing high speed strategies enough to determine if there is a similar tool path available, I always default to the Volumill strategies. In Camworks it likes to spiral ramp down and then HSM a channel to the edge of the pocket and then it follows the same path as the fusion so it isn't ever changing WOC such as fusion does when it steps out for the next widest ring to cut. It used the precut channel to make its outward move and then engages the next ring out at the same stepover it left the previous. Probably not a big deal with a huskier motor, but my BLDC always bogs when re engaging which made it a less comfortable method for my setup.. I'm curious to see of the new AC motor makes a difference there.

Hoping to have the new motor j stalled over the weekend. Will see then I suppose!

Sent from my XT1080 using Tapatalk

[lcvette]

Peter, have you played with the feeds and speeds yet?

Sent from my XT1080 using Tapatalk

[ChrisAttebery]

I bought a Best Carbide 3/8" 3 flute 45 degree flute end mill on my way home yesterday. I cut another batch of the rings in my last picture today. They are 3/16" thick and have a 2.8" ID. I used the pocket operation at 4500rpm, 40ipm, .1875" doc, .200" WOC and 1.5"/min MRR. I had to crank up my mister because the tool was loading up at first. Once I had enough coolant flowing the mill was happy though. I think that's about as hard as I'd like to push the machine. It chattered once in a while, but not so bad that I felt like I needed to slow it down.

I was taking the finish passes at 60ipm and the finish looks great. These were really light cuts though, .010" X .375" or less.

[lcvette]

Sounds like you are getting there!! .200" WOC is really close to that bad zone between the middle of the tool which is probably why you were having some chatter. Stay away from the 40-60% stepover region of the tool, better to go deeper then be in that zone. Or with such a shallow cut you really could drop down to like 40% and increase feed rate a bit.. Shallow cuts are tough because the feed per tooth should be a good bit higher because the endmill is engaged for a shorter distance on the flute, that also means that generated heat has less time and less chip to pull heat away from the tool which is why you needed to bump up your cooling system flow.

A more dialed in formula for that cut would be:

4500 RPM
.15" WOC (40% stepover)
.1875 DOC
54 IPM
.004" FPT
1.52 in³ MRR

That gives you the same 1.52 MRR but will be even happier under the no mill zone without any chatter and the surface finish should look excellent!

Chris


Sent from my XT1080 using Tapatalk

[ChrisAttebery]

Like this?

https://youtu.be/T_Gjc9ICF2I

The machine is definitely happier taking a narrower WOC at a faster feed.

A more dialed in formula for that cut would be:

4500 RPM
.15" WOC (40% stepover)
.1875 DOC
54 IPM
.004" FPT
1.52 in³ MRR

[lcvette]

Are those with the settings above?

Sent from my XT1080 using Tapatalk

[lcvette]

It looks good to me.. I'm not used to seeing the corners cut like that. Usually adaptive will round the corners first to make that transition really smooth and not so harsh at that 90 degree move.

If you don't have it. I recommend getting FSWizardz I have the pro version on my phone think it was like a one time fee, wasn't too bad and definitely worth it. It has saved me so much time setting up programs and I have come to really trust its suggestions. The key is to use it for your machine. So if you set your max RPM and enter in the other data for the cuts it keeps the geometry of the cutter at its most effective.

For me I set pretty much everything up for 25-30% stepover on my .5" DOC and deeper and then just adjust my feed per tooth until the mill is happy. It kicks out the new IPM based on those days points along with the material and cutter information.

If you notice in your video, you have a nice steady smooth stream of chips being ejected, that is a sign you are getting dialed in. No chip recutting. Good MRR and can chew through your part times alot faster without killing the machine or cutter.

Keep it up, looking good!

Chris

Sent from my XT1080 using Tapatalk

[petemilligan]

Peter, have you played with the feeds and speeds yet?

Yes - started as stated. Backed it down a little to 650mm/min because I'm chicken. I'm flying through the project now.

No more tinsel (The original problem where buckets of it were being produced). I have chips with mass!!!

Thanks for all of your help.

Cheers,

Pete

[lcvette]

Glad to hear your rolling through your jobs! Get some video up for your readers if you get a chance!!

Sent from my XT1080 using Tapatalk