Hi Folks, I'm looking for some advice to improve the quality of my parts. Today I machined this, its aluminium, 80mm diameter, with 0.5mm deep pockets. It was modeled up in SolidWorks, run through Mastercam to generate the g-code, then run on the mill using Mach3. I have an X2 with CNC Fusion screws and brackets and a Kelling 3 axis driver and motor kit. I've had the machine for a few months and am getting more confident with it but I'm a noob when it comes to the details of the software and I'm still learning the tricks of machining.

This part was cut with a 2mm diameter end mill, feed rate of 50mm/min, cutter speed around 4000rpm. I did it with a roughing cut 0.35mm deep and a finishing pass at the final depth (overkill???). Each pocket was finished before the next was started.

Problem 1: The red boxes show the typical problem I'm seeing. The edges of the pockets are wobbly and in some cases it is almost like the cutter is not following the tool path correctly. The U shows a great example of the problem. The two inner "vertical" edges of the U should be parallel with no jogs. The two L's should also be identical but the left one also has a jog in the edge. Other areas I've highlighted are just plain rough.

Problem 2: Where the tool path is drawn as a curve or elipse in SolidWorks, it is coming out quite rough and faceted. Any thoughts on software settings to improve this?

Problem 3: The two 4.5mm screw holes came out almost as squares with rounded corners, even though the tool path and g-code shows a circle. When I ran a drill through them a significant amount of material was removed.

I checked for backlash today on both the X and Y axes. I used my vise and DTI and moved back and forth 100mm from the vise face. Backlash seems pretty good although the repeatable accuracy seemed to decrease as the feed speed increased. I had the machine rapiding at 2000mm/min but over about 1000 it looked to have a potentially noticable effect. However, there was no rapiding during the cutting of each pocket, only when moving from one to the next.

Sorry for the long story and big pic but I'm hoping someone can help to shine some light on these problems and confirm if it is software, hardware or both.

http://i91.photobucket.com/albums/k315/cloted/Wobbley15.jpg

My first impression is it's a software problem.
If it was backlash or losing steps rapiding between letters,
I don't think the letters would be as inline with each other as they obviously still are.
You could try running your program through a simulator and see if the finished results are the same.
I like using the demo version of Flashcut CNC (http://www.flashcutcnc.com/html/dow.html). They have version 3.0.7 available now.
Setup the Tool Table Config with your endmill size and you can watch it run the code.
Would be easy to see if the U and L are machined correctly.
If so, then you can look at mechanical trouble.

Looks like you need to use a smaller diameter cutter, that would explain how it bumps out on the edges like that. I would also use the engrave module of Mastercam. I would also check out your tool params in Mastercam. Maybe slow the feedrate for the tool itself(Mastercam has built in tool feeds for each tool) . Also I can't remember exactly how but in Mastercam looks like you need to adjust maybe the way the tool enter and exits the lettering. Does it make the same letters in the preview in Mastercam? If that don't work then I agree with Hoss.

Agreed with some of the comments above. I'm not sure a smaller tool is going to help much though. Some of the features you have there really look like backlash I have to say. Big flats on axis reversals etc. Possibly try measuring the backlash while putting some load on the table with your hand? There might be some float in the bearings or mounts that don't show up under no-load conditions. Also check your head is not loose on the gibs and moving side to side.

It could also be due to poor geometry in the model, such as a lack of trim where surfaces meet, hidden overlap, etc. Do you have a method of extracting the edges of the surface geometry so that you can observe the geometric constraints that the toolpath will follow? It is usually easier to see the modelling errors in the form of poorly trimmed 2d entities.

Thanks for the thoughts guys. I don't think there is any issue with the surfaces as they were sketched and extruded in SolidWorks, not imported (assuming that the translations between programs are working correctly).

Will try simulating the program to see if it runs OK (that should help identify if curves are being poorly approximated).

Will also check for backlash under load. The X and Y gibs are nice and snug. Haven't checked the Z for a while...

The pockets are all at least 2.1mm wide at the narrowest point so I would expect that a 2mm cutter is fine for the geometry. I set the feed rate myself and the machine ran fine with no visible stress/overload.

I'll post back as the investigations continue...

How long is your cutting tool. Are you getting tool flex of some sort?

(forgive me if that's stupid)

Thanks for the thoughts guys. I don't think there is any issue with the surfaces as they were sketched and extruded in SolidWorks, not imported (assuming that the translations between programs are working correctly).

It might not be Solidworks' fault. If the text was translated from one of many windows fonts, there are lots of those with built in errors and poor trim.

Cutter is 2mm long for about 10mm, then tapers out to a 6mm shank. Should be alright with aluminium I would have thought.

Good though about the font (seen that many times when modeling at work) but its lines, arcs and splines, not font text. I couldn't be bothered looking for a font so just traced over a graphic inserted in a sketch.

Do you have the Sherline Mode "Sherline 1/2 Pulse Mode" enabled in the
"Port Setup and Axis Selection" located in "Ports and Pins" in Mach3?

This is important when using the Keling 4030 drives.

Jeff...

Also check the
1- The tool runout
2- Backlash
3- Increase your Feed rate a little (if it is actualy 50mm/min)and use any mist/coolent. If your feed rate is 50mm/sec then its too high.
4- Check the Steps/unit setting for all axis in Mach3.
5- Reduce the spindle speed to 2500~3000
6- Check for any loose stepping , this may be due to using low voltage /perage powersupply.

Another reason may be, the holding arrangement of your workpiece. Check the holding/clamping is tight enough against the cutting forces..

Wow, you guys are awesome! I leave the PC for 45 minutes and there is even more advice waiting when I return.

Anyway, first points to LongRat, the Z gib screws needed tightening. She is now nice and snug on all 3 axes.

Hoss, ran the simulation in FlashCut and the U and L look fine so I'm guessing the code is not the problem. Hmmmm...

Jalessi, yes, I have "Sherline 1/2 Pulse Mode" enabled (that was the last setting I discovered when trying to get the machine running to begin with)

Khalid, sorry, feed was actually 60mm/min and I cut with CRC. will check the other settings when I get a chance.

Have you checked for a sloppy spindle (negative preload).

Phil

Hi Clot.

I do very similar work to yours on my Syil X3 in 6082 aluminium. Not sure how robust the X2 is compared but I've posted you a .tap file (zipped) of a BUELL logo that I use, it will fit inside an 80mm dia but use a test piece just in case.

P.S. This is not the 'actual' file I use so check it, check it again, then once more before you use it.

All my code is metric.

X0 Y0 is the centre of the piece, Z5 is the safe zone. F30 is the plunge speed with F60 as the cutting feed, it will cut the whole 0.5mm deep in one pass, you may wish to alter these to suit the X2 but they are well within the capabilities of my X3 with carbide tooling. As it is, this file takes 25mins on my X3 but you could further edit the plunge from safe to +0.5mm to speed it up. I use parrafin as a coolant/lubricant using a brush to apply it & wipe away any chips.

On my X3, this logo cuts perfect & accurate, it uses a 0.30 stepover on the 2mm tool which gives me a machined surface that will easily polish out. If it's any differant on your machine then look towards hardware rather than software.

The initial code is generated by Artcam Insignia which I find really easy to learn & use. You set the workpiece dimensions then import a scaleable vector onto it before generating the toolpath. I have succesfully engraved many logo's this way & find it very easy to modify for differant sizes, applications etc.

With regard to the 2x screw holes, personally I'd drill them. When making similar items I place the blank on the machine, set the X0 Y0 then perform any drilling, profiling, engraving etc using differant files for differant tools. It works for me & my set up, I'd love an autochanger & flood coolant on demand but I feel I have much more control this way & it makes it a lot easier to modify to differant parts.

Please let me know how you get on with it & what other items do you make???

Sweet, cheers for the file. Looks good, I'll give it a go in the weekend.

So far I've done some indicator block off plates for my XB12R (running 1125 mirrors with indicators), a couple of timing covers (which ain't so good) and some engraving on some computer covers for a friends business. Gonna do some more parts for the bike once I get the hang of the machine and get these bugs ironed out. I've got heaps of tweaks to try thanks to the forums and I hope to re-cut something this weekend. I'll keep you posted. That program will be a good comparison to check out my machine settings, accuracy and also get a feel for how I should program this type of part.

Hey Clot, I still thinking Mastercam good be the suspect. For Xmas I was making my friends engraved plaques when I had a couple of 'em screw up kinda like yours. At first I thought it the file was messed up, but the preview was perfect, then I thought it was resonance. But upon further examination of the preview especially fully magnified, I found hundreds of little dots in the font that you couldn't see at on the normal preview, and the machine was trying to cut those little dots. Got that resolved and I found another problem was even through I set the feed rates , Mastercam had individual feed rates for each tool you selected. I corrected that and my problems went away.

OK, so I ran the program from Babba today after tweaking some settings. The cuts are much improved (although my cutter might be a bit worn) and the wobbly edges have almost disapeared. Thanks to all who offered their advice. It looks like there were several machine issues that are now sorted. Hopefully I'll get some time to try my own programs tomorrow and see if there are any software issues too but I'm much happier with the part quality now.

http://i91.photobucket.com/albums/k315/cloted/Improved15.jpg

Thanks again guys!

I have had similar problems with computer generated code. If I have a weird problem the first thing I do is read the code myself.
I know many people don't read G-code all that well (myself included) but there is still a real need to know what the code says. If the code is computer generated and then computer checked in a simulation program, what is to prevent a bug from making it look okay in the simulation? I had the machine just make an odd cut in the middle of a straight move. It looked good in the cad program and looked good when I converted it to G-code but the problem was still there. I looked over the G-code with a list of codes in my hand and a found the problem, it was coded to do the move it was doing. I went back into the cad program and under high magnification lo and behold the line was there. The program was doing exactly what it should do but it took quite awhile to find it.

Mike