Hi All ! I need an advice, please I am going to mill some aluminum plates for my new CNC router. Can anyone give me advice if this material is good for that purpose 1/4" thick .25" CAST Aluminum MIC-6 PLATE 7.875" x 24" long QTY 3 sku 136618 | eBay and if not which aluminum is better for this task. Thank You in advance
This is probably the most commonly asked question. The quick answers is 6061 T651 is a rolled and heat treated plate that gets it’s physical properties from the chemistry, the rolling and elongating of grain structure, and the heat treatment process. A Cast Tool & Jig plate is produced by casting metal. There is a homogenization process that helps with grain uniformity, but there is no secondary rolling or quenching process. The 6061 T651 Aluminum plate will have residual stress as a result of the rolling and heat treating process, but also has higher strength. The Cast Tool & Jig plate products are much lower in strength, but also much lower in residual stress. Most Cast Tool and Jig plate manufacturers guarantee their specified flatness even after machining the part. If there is a need for strength in your part design, then you should not consider Cast Tool & Jig, plate. However, if strength is not a concern, Cast Tool & Jig plate will offer much better dimensional stability and flatness to your finished part. so with that in mind this might be better.... 1/4" thick .25" Aluminum 6061 PLATE 5.125" x 24" long Pieces 3 sku 137025 | eBay Bob
Thank You, Bob, for so in detail explanation. Strength and flatness wise everything is absolutely clear. But I suppose, some strength deviation of different aluminium alloys in our case, (making plates for little cnc router) is not principal thing. When I asked which aluminium is better for cnc plates I mainly speak about machinability of material. It is absolutely clear that CNC router is not an ideal machine to mill and cut aluminium, however in some circumstances it is close to possible. In my case I have C-beam CNC router and I am going to cut plates for another CNC router on this machine. So, I am mostly interested which aluminium is more CNC router "friendly" in terms of cutting and milling ( easy cut, clean and shine cutting surface and so on). Thank You one more time. David
c-beam will cut either no problem. Finish will be better on the rolled 6061, but the cast will cut a little easier. for end plates on say an ox either will work just fine. Bob
Wow! That stuff is expensive. Do you have metal yards near where you live. I pay $3.50 per pound at a metal yard. That plate would cost me about $16.98 (3.636 pounds/ square foot for 1/4 inch MIC-6 at roughly 1.33 sq feet). Of course that is if I found one that size. If it needed to be cut, there would be an additional $3 charge. What I do is figure out roughly what I need and look for a piece that I can fit all the parts on. If it is still a bit big I get it anyways because it saves the cutting fee and I know I will find a use for the left over. Maybe I need to start my own online metal shop.
Expensive?!?! It depends. How about this Openbuilds Kyo Sphinx C-Beam CNC Router Plates Stainless Steel Extra LARGE | eBay It is exactly what I am going to cut. To cut once! It is not my business to cut aluminium plates. I would like to cut that plates once , to assemble Sphinx CNC router and use it for cutting fiberglass, carbon fiber, plastics..... (99% of times). Very rear aluminium and cupper. (1%). So, with 1 of this 3 expensive sheets of aluminium I can cut this whole set and it will cost me USD 20. vs USD 200 + . Do You think it has a sence? David P,S. Oh, I guess You thought, that USD 44 is the price for 1 sheet, No, there are 3 sheets in lot
it show's 60 with shipping for me. Just do yourself a favor and look up metal sales in your area and give them a call. Bob
Yes, exactly 60 for 3 plates, so 1 plate is USD 20. In my area My area, Bob , is Georgia. Not US state, but Georgia Caucasus. Too difficult to find something like this here. Impossible . So I have to buy it from US David
I just googled it don't know what city you are by but this came up. Georgian Metal Impex, Tbilisi, Georgia I do understand it's not as easy to get metal in other countries as it is here in the states. might not be worth the time and energy to chase a better deal... be sure to post some pictures when you get them machined!! Bob
So, here is my first cut of 1/4" cast aluminum MIC 6 I used 1/8" spiral "O" Flute bit (Shaft 1/4") from Toolstoday.com Feedrate was 10 in/min spindel Bosh, about 11 000 RPM pass depth: 0.015 in Use cutting fluid I can not say that I am happy with the cut. Typical DIY quality, not professional, shine cut at all. Sure, it will be absolutely ok for CNC router which I am going to assemble. But from professional point of view quality sucks. May be it is principally impossible to make shine cuts by cnc router? I don't now, may be somebody say it. May be it was wrong bit, or wrong speeds and feeds? If somebody has any idea how to make cut more clean and professionally looking, will appreciate the advise. David P.S. And one another question. The edges are sharp enough, so I rounded them by sand paper. One more DIY result. Can somebody help me to advise how to make round edges (make chamfer) using cnc, which bit to use for this purpose and which profile. Thank You in advance
They are called chamfer mills (eg. 2 Flutes Carbide 6mm Chamfer Mill 90 Degree HRC45 End Milling Cutter Router Bit | eBay )
Thank You, Darathy. The question about how to improve cutting surface quality (which bits, which aluminum, speeds and feerdates and etc) still remains open.
I would be aiming for a chipload of around 0.076-0.102mm for a 1/8th up cut single as a starting point. At 11k rpm I would also aim for around 800-1100mm/min feeds. Getting a nice cut in aluminium on an Ox is not hard but extra steps need to be taken to get the best results. Expecting the exact same results as an expensive and heavy commercial build a little unfair as thou shalt not ever desecrate the CNC holy trinity. Performance, Cost, Speed.... Pick two In saying that my desktop size Ox setup with double belts give sweet results if I understand that the lighter machine has to take more time to cut out a part compared to the big CNC routers I have had access to in past jobs. Some tips to help: measured the runout on your spindle/router? Any wobble in your setup will show as chatter. Ebay spindles are good value. 800w is the largest I would put on an Ox style build as it to me is the best power to weight ratio that suits the forces an Ox frame can deal with Made sure your stock is held so it can not vibrate? Any movement will show up as chatter, a simple vac bed and double sided tape is a good mate to surface finish. DONT recut chips. Bogs your cutter down, smears and over heats the area so make sure to have a good dust shoe and double points if you add a compressed air blast/mister Onion skin cut your parts. Rough out your parts in small step downs with an older cutter leaving 0.25-0.5mm off the final target wall size and floor, clear all chips from the table and then swap in a new cutter for the finish pass that hits the full wall cut depth to give a cleaner edge. When your finish cutter gets ratty, retire it to becoming a roughing cutter The cut I get are not as good as from a commercial shop but my ox cost about a 20th the price and gives results that are dimensional accurate ( it can remake Ox plates that have good bearing fit and wheel alignment) so I am very happy with huge VALE you get from an ox. I have attached some photos that give you an idea where I stopped trying to make it better at. I would get better results if I added a spindle (This was cut with an RC outrunnner motor spindle) and vac bed but to be honest I am not sure I will bother right now as I am super happy with it as is! Hope this rant was helpful!
WOW!!! Sure? 1100 mm/min !! It means 4 times more speed then I run (254 mm/min) Please Please confirm feed rate for cast aluminium MIC-6 plate Thank You very much for Your advises. David
If you know the tools recommended chip load you can use the below calculation to find a ball park of where to start testing your feeds and speeds at. Chip Load = Feed Rate ( millimeters per-minute) / (RPM x number of flutes). I can confirm that I was running a single flute up cut at 900mm per min with the spindle at 13000rpm. I would run half the speed if I reduced my spindle speed in half and would double my feed if I swapped in a double flute cutter as examples to help show how these three variables all need to be kept in balance. If you have been running at 254mm per min at 13000rpm then I would suspect you may actually be killing your tools faster than if you rampped up the feed speed! When you move too slowly or you spin too fast the tools cutting edge can not bite the work and the trailing edge ends up rubbing the material away. Rubbing causes the heat that would be ejected with the chip to sink into the stock and tool. A rubbing tool will also soften the leading cutting edge that will also become dull much faster than when you maintain proper chiploads. check out this image from CNCcookbook.com that shows BOTH tools striking with the leading edge (yellow line) striking to high into the work and rubbing (was an image comparing a standard tool and micro tool in rubbing situations..
Thanks a lot for in detail explanation. I will try today this feed rate. You mean 13 000 RPM, not 1300 , do You?
All newbie CNC operators are encouraged and advised to "understand chip load". "If the tool is not moving fast enough forward for the speed its spinning, it is doing more rubbing than cutting." Ideally--and this was the thesis behind "chip load" in the first place--the chip created by a cutting tool carries out with itself the heat generated in the process of creating it: if all the heat goes out with the chip, the cutter stays cool. Newbs tend to be both timid and too conservative, thinking they are saving their equipment by "tip-toeing" through the material and thus, "not asking as much it." In the end, they are asking it to die of heat stroke. :^) Confession: I am a former newbie CNC operator myself. I have recent crownt myself a middlebie.
