Not having the CV set right usually causes rounded outside corners instead of being sharp. CV Dist Tolerance tells Mach how far away from the corner it should start slowing down. Can't really say what my settings are right now due to both machines running code but I think my stop CV is set for great than 90 degrees. Tuning the acceleration on the motor especially the X and Y to something along the lines of 15-20 will give smoother results and less shaking of the machine, I think my z is set to around 35 otherwise it slows down 3D cutting.

Try reducing your bit stepover to 8-10 percent and you'll get very smooth results with little to no lines.

Looking great though, have you tried cutting any rfl files yet?? I believe I have a few 3D files I can send you if you'd like trying them out...

Gerald

 

Great to know it's not a mechanical issue, just a software problem, those are usually easier to fix. Looks great, what bit did you use?

I'll send over a few... I've never used ArtCam, does it support grayscale reliefs also? I have a ton of those as well...

Gerald

 

I might just have to take another look at ArtCAM !! Very nice work !! Looks like your using a raster toolpath, if you change it to offset toolpath where it starts in the middle working its way out you'll eliminate the choppy marks around the border..

 

Oh I see, Aspire handles it a bit differently where the text and relief image become one component, I would rough it out with a .25 ballnose and finish cut it with either a 1/16 or 1/8 tapered ballnose bit... Looks great anyway though !! 1 hour isn't bad at all. The Harley signs I do run .5 hour for roughing and 3 for finish, but no sanding required, just touch up some areas, stain and poly....

Keep it up Neil, looks great !!

Gerald

 

Hi Neil, a great series of hints on how your have gone with your Frog.

I am just wondering if you have used it for working with soft metals such as Aluminium and Brass, and if so how did it handle it. I am curious because I note the discussions about flexing of the gantry, using the open build extrusions. I am actually resurrecting a stalled build from a couple of years ago where I acquired a lot of 80x80 and 40x80 extrusions which I am hoping to incorporate, rather than buying all new stuff

Cheers

 

Try these bits out Neil, I was pretty skeptical but I keep the rpms about 13000, feed 20 and DOC .04 ramping into the cut they work ok. I cut a full set of plates from .375 6061 over the weekend with one bit... Here is the secret i've found to cutting 6061 (brass is easy) direct a compressed air nozzle down at the tip of the bit and when doing profile cuts spray every second pass with WD40... works like a charm but keeping the chips blown out is the biggest thing, otherwise they like to reweld in the cut.

http://www.ebay.com/itm/111563788736?_trksid=p2057872.m2749.l2649&ssPageName=STRK:MEBIDX:IT

At 15 bucks with free shipping can't lose and you get 5 !!

I use bits from ToolsToday as well, pricey but great quality.

Gerald

Here are a few photos of my air blast/mister setup on my big machine,

 

Only problem with that Gray is as the bit moves in different directions chips get thrown out going different ways, it would have to be a hell of a vacuum. Plus I think having one air nozzle is bare minimum, you really need 2 facing in X and Y directions. Profiling parts is where I get the most chip weld, with one nozzle the chips don't get evacuated very well when going sideways to the nozzle direction. Also i'm not too comfortable spraying flammable liquids and having a Vac suck them up, shop vac would probably go boom. WD40 does wonders at reducing chip weld and improving the cut quality.

 

Treat the MDF with a wax to prevent it from sucking up WD40 and the likes. I use liquid beeswax on all work surfaces. To prevent sliding use a bit of salt under the work piece (if you use the vacuum table).

 

I have the same issue, my bed is 3/4 ply with 2 layers of MDF on top. I just add another piece of MDF larger than the piece i'm cutting, it soaks up the WD40 pretty good and leaves the bed underneath dry... I thought about building a box with 6" walls to to help contain the overspray.

I spray my bed with shellac after surfacing, but that doesn't last long when you get alot of cuts into it...

LOL i'm thinking of a third machine, maybe a laser cutter..

Gerald

 

While I have yet to finish my CNC router I have cut lots of aluminum dry on mills. You can do it quite easily with the right tool and air blast.

I typically used solid carbide 2 flute high helix TiN coated end mills. Air blast on the tool to clear the chips and climb milling. Keep the chips light and thin but large in size. I liked curls the size of my small finger nail with a little curl to them.

Certainly flood coolant is historically preferred in most cases but more and more we were moving to tooling that was cutting dry. This included 3" face mills through pre hardened steel at nearly 300 inches per minute.

 

What are the feeds and speeds your using to cut say 6061 with the 2 flute? I have a few high helix 1/4" end mills designed for milling aluminum but still have issues with chip weld when I cut dry.

Gerald

 

The old prototrak was not high speed so speeds and feeds were low. Probably much lower than what is typical with the routers used in these OX builds.

It has been more than 6 years since I regularly ran any equipment so my memory is fuzzy. I did a fair bit of manual cutting in the 1700 to 2200 rpm range and 10 to 25 IPM. This was on mostly 1/2" and 3/4" tooling. probably in the .005" to .007" per tooth chip load range. The production stuff was much higher chip load but we were still running flood coolant on aluminum in the production horizontal mills and lathes.

 

I think that's actually part of the problem, the rpm these routers turn. With common routers it's difficult if not impossible to get your rpms slow enough where you don't have rubbing. Some of us have variable speed routers but even my 3 1/4hp Porter Cable goes only as low as 10,000 rpm, but at a cost, it loses alot of torque. From what I understand usually about 4-5000 or lower is a good range with 1/4 and 1/2" end mills. With smaller bits you can run higher rpms and keep a good chipload, but when using a larger end mill like 1/4 or 1/2 the rpms need to come down a lot or you'll start rubbing and melting the aluminum instead of cutting.. I have found with a 1/8 O flute end mill 13000 rpm with 20ipm and a .04 DOC climb milling works pretty good, no broken bits.

I use mostly "O" flute end mills designed for higher RPM routers and they seem to work pretty well, just much more costly than a solid carbide 2 flute... I can run these dry on everything but slotting operations (profile cuts) or deep pockets, that's when I break out the WD.. I have seen a few people run 1/4 end mills with just a mister moving fast 24k rpm at 120IPM .06 DOC, but on rigid machines with 10hp spindles.

Check out NYCNC on youtube, he has alot of good info on milling aluminum... Or Toolstoday...

 

I personally haven't but a lot of guys over on Joe's CNC forums have, no one has anything bad to say about them. If I decided to stay with a router I would go that direction, 5000 rpm and the ability to control it from Mach 3 is appealing.

 

Good move changing to the Gecko G540 Neil
If you motors are getting hotter than 60 deg.C then consider changing the current resistors (as per the Gecko instructions).

Tweakie.