[xesxes]

Greetings all,

My name is Travis and I am new to the board and CNC in general. The company I work for has recently purchased a Roland MDX-540sa with Rotary a-axis, and we are having a bit of trouble with Aluminum and some other materials and was hoping that someone here might be able to set us straight.

simply put, it seems that everything I put in the machine runs for a time and then I run into some sort of overload fault, whether x, y or z. I have seen this machine tear into aluminum like a champ with no problems, and other times it stubs it's toe and starts to cry. I don't get it.

It feels like if where to try and run a job like this I could not.
[ame="http://www.youtube.com/watch?v=ejLVRmp5mck"]YouTube- Roland MDX-540 milling aluminium keypad[/ame]

also the roland software doesn't have very good plunge control, I can't seem to find a way to change plunge vs feed. every fault as occured right after a plunge.

sorry for the long winded and scattered thought post.
hope someone out there knows my pain.

Thank you,
-Travis

[matto]

hey travis,
I have a 540 and 650 roland machine and have cut alot of aluminium , first off I am not an enginneer and love these machines for the ease of use . I think it comes down to the basics of machining and finding the happy equation between the alloy , the cutter (flutes ,coatings , type) and then the feedrates . I presume you are overriding the presets the roland software are calculating as these are typically conservative. I also add a bit of cutting lube from time to time . Can you post more info ???

[xesxes]

I have tried messing with them a little bit, but even the default settings are giving me issues. How often you do add the lube? We currently have an air line set up. Here is a picture.



I am also finding the the Roland software is pretty horrible. Looking into Mayka. What software do you use?

Thank you for any help you can offer,
-Travis

[mactec54]

Hi xesxes
What cutter size, feeds & spindle rpm are you running

[matto]

hi , thats useful to see a pic , i take it that that is aluminium , not a chemical wood ( just wondering due to the dust ??) . If it is ali , then one issue you face may be the depth of vertical plunge against a vertical wall ?? either do some cad work on the object you are cutting which is a work around due to the limitations of the roland software i.e control is only region and depth , can you put some taper on those walls . Another trick is to cut to depth with an offset , therefore you end up with a stepped taper?? I am still with srp ver 1.17 but are looking at mayka , rihno cam , and a friend tells me sprut cam is good . It may be worth looking at vetric software too.

[awerby]

All endmills are not created equal. Some are designed to plunge straight into a piece of material, and others have a hard time doing that. It has to do with how it's ground on the end, in the middle, and whether it has a drilling action. There are drill-mills available that have an actual drill-type tip, that might make this work a lot better.

All aluminum isn't the same either. Pure aluminum is rather gummy, and tends to trap the end of the cutter. Lubrication helps with this to some extent. All aluminum alloys need lubrication to keep chips from welding themselves to the cutter; you might be able to provide this through your airline by putting an oiler inline - these are commonly used for lubricating air tools. And using the right aluminum (I like 6061 T6) helps a lot.

The CAM software you're using might also be too simplified for what you're trying to do. When cutting metal, it's usually better to "ramp" into a cut, descending in an inclined plane, rather than plunging straight in. And if you do plunge straight in, it's better to do that at a slower rate than the horizontal cutting. Most CAM software will let you program that in. Take a look at VisualMill, if you're shopping around for a new CAM software package. It's pretty economical if you get the regular version, and if you need a lot of advanced features, there's a Pro version you can get that is considerably less expensive than the competition.

Andrew Werby
www.computersculpture.com

[xesxes]

Thank you all for the help. Today I started another aluminum project at work, one with a deadline. Currently the machine is sitting still due to some sort of problem I cant tell through the webcam. I am cutting 5/8" inch mic6? aluminum from McMaster. I am roughing with a 3flute flat EM, and have only made it about half way through the material with all the overloads and restarts. So stressful I want to punch a wall. I keep reading how amazing the Roland is but at this moment I want to destroy it. argh. Sorry for ranting.

I am cutting @ 57ipm with a depth of .05 and a stepover of .07 (i think).

would anyone beable to list the best endmills to use with the MDX-540 and aluminum from McMaster?

Matto, in that picture I am using RenShape. RenShape is pretty easy. what is your typical Aluminum workflow? rough method, feeds/speeds, finish methods, stepover and stepdowns.

Also we bought RhinoCAM 2.0 along with a CNC router but I am working with it on the Roland as well. We are looking to purchase PRO if I can get the machine to produce results.

I am literally at the verge of tears. It seems that all my boss wants to run is aluminum and I have no idea what I am doing other than wasting the company a ton of money.

[matto]

hey , xesxes
I can hear your pain . I am sure you will get there , the frustration is that it will not be a singular fix , but a number of factors , so rest assured there is no magic cutter , or feedrate ratio that everyone knows except you . Lets start with the file you are cutting can you send it to me to take a look at , you might want to send just a segment . I will take a look at it in srp player and offer any clues . Can you send a .sat file ??? if not try iges or dxf ver12. [email protected]

[MrWild]

It pays to have machinist experience. Failing that, speed and feed charts are your friends. You are just blowing air? No mist coolant? No flood coolant? That's a fail right there. While the video may show no apparent coolant, there may be a spray mist you don't see. It also looks like you are using uncoated high speed steel end mills. How much step over are you using for your plunge material removal? Have you thought of clearing material by just taking .05 deep pocketing passes?

It sounds like poor cutter selection, with no coolant, along with too high of feeds. The cutters load up, can't clear chips, and the machine stalls. Operator errors, not machine errors.

[Willyum]

A few points in no particular order...

Notice in the video that they are only taking .005-.010 Depth-of-Cut (DoC) while running that high of a feed-rate!

57ipm with a depth of .05 and a stepover of .07, seems very excessive for this style of machine no-matter what spindle speeds you are running. It sounds like the machine is hitting its limits and alarming out...? Also, Straight Plunges into material should be 1/2-1/3 of regular feed rate.

I'm assuming you are using a 1/4" EndMill(from pictures)? High-Speed-Steel, High-helix, center-cutting, with 2-3 flutes would be optimal for aluminum.

Start slower and then work up to finding out what the machine can handle. A good starting point might be:

1/4"-3/8" HSS 2Flute EM: 1500-2000rpm .02-.03DoC 10-20IPM (Without Coolant but occasional WD-40 spray)

Get the program to complete the run, or plunge, or difficult part of the program. Then next time ramp it up a bit.

Hope this helps,
Will

[macsgalicia]

Roland Machine User MDX EGX JWX DWX- ArtCam, RhinoCAM, Enroute, VCarve Pro, try to contact me at [email protected]