Asheville Makers Wiki

You've loaded an old revision of the document! If you save it, you will create a new version with this data.

Here are test some comments on a workflow to get a cutting file for the MicroProto mill. I am happy for this tool to be on essentially permanent loan to the space.

The mill itself is a MicroProtoSystems DSLS3000. http://www.microproto.com/MMDSLS.htm
It can accommodate pieces with X = 12", Y = 5.5", Z = 6" and they claim a "Position increment resolution" of 0.000125 in with a mechanical repeatability of 0.0005 in.

The original documentation is in the green binder.

I am not really up to speed with Fusion 360, and I am very rusty with the whole CAD/CAM process. But now the mill is running again I want to get back up to speed with it. As Fusion 360 is what several people are working with I thought I'd try to figure out a workflow starting from there.

Most of the problems I have had getting files ready for the mill usually seem to end up connected with some sort of scale issue.

Fusion 360 does have an option to write a Mach3 cutting file. When I have tried this I get a file that has cut limits in Mach3 that are ridiculous (a 2" x 2" piece may show a cut boundary of 10,000"). Steve has figured out which lines in the G Code seem responsible for this, but I think hand-editing a G code file is a risky habit to get into. And there are lots of other ways to "get from here to there."

So, in Fusion 360, make sure your part is sized in inches. There are probably several ways to do this, but my few tests resulted in a part being created in mm. If you mouse over the units block it will give you an edit icon and allow you to change to inches. It seems even if you create in mm it will handle changing the units for a finished model. I think it's worth checking a few measurements to make sure everything looks good.

Zak clued me in to writing a .stl from Fusion. This option is in the "make" tab. Probably more than one way to do this, but I box selected the whole object and then picked 3D print from the make tab.

It seems that you need to pick something in the refinement dropdown (even if it is the same option) to get fusion to build and display a mesh. Uncheck the send to 3D print utility box and when you click OK it will prompt you for a .stl filename.

Move this file to the mill computer, open MeshCAM from the desktop, and load the file. It should give an info window telling you the piece dimensions and that it is working in inches, and then it will prompt you for the kind of work you are doing. I have only used 3-axis.

Meshcam is pretty easy to use. In the toolpath just work left to right and in moast cases the defaults will work. The first 3 will usually be fine. Righmost on the first row allows you to pick your origin. Usually bottom left or center. Whatever you pick for this has to be the same point you choose to zero the mill when you move on to Mach3.

Max cutting depth must not be deeper than the length of the mill (the cutting bit) you will be using. Machining region allows you to only cut part of your stock (again, pay attention to depth). And then the fun one...

Generate toolpath looks complicated but it's not as bad as it looks. But let's start with the tools part. For any phase of the cutting you can select a different tool (the tool I think is technically "the mill" - end mill, ball mill, etc-- and the machine is the milling machine, but it's easier to refer to the cutter as the tool (or the bit). If a tool isn't in the list you can create your own, and although you can override the feeds and speeds in the cutting path dialog, you need to put some in when you create the tool.

Page 51 of the front section of the green binder gives some generalizations for how to calculate feeds and speeds for different materials. But as I understand it you need each tooth or blade of the cutting tool to remove between .004 and .008 inches of material (page 54) with a table on page 53 showing where in this range you need to be for different metals. From that point you need to know how fast the cutting edge is traveling (from spindle rotation and tool diameter) and from there you can figure out how fast to move the tool into the material to get the right chip size. I'm sure some CAD/CAM software figures this out for you, and there are lots of websites that help. I have (mostly) cut wax and wood so I have not had to worry too much about getting this exactly right and I just pretended everything was aluminum on the assumption that if I was working too slow the materials I was using would not destroy the tools from overheating.

-- If you try to cut too fast you will either break the cutting tool (usually cheap) or the spindle pulley (ditto). As I understand it, cutting too slow in metal makes the cutting edges "rub" rather than cut, which generates heat and the  tool then becomes dull.

Once you have the tool you need available, the left side of the generate toolpath dialog is the roughing phase. You can select what you wanbt to do with the checkboxes, and run just roughing and then see what the generated path looks like. Then you can select different finishing options and see if they seem right. For getting smooth contours, the parallel X or Y options work well with a round nose mill. The finer you make the stepover the better your results will be (say 1/5 of the radius of the tool) but the longer it will take. Waterline and pencil finishng seem to work best when you have features that have more sharply defined contours from a background plane.

You will end up with something that looks like this. Here there are 3 phases, but they are all shown as overlapping lines. You can check and uncheck the boxes for the different operations to see more clearly what is going on. A "Gotcha" here is that when you click save toolpath it will only save what you have checked at the time, not everything that has been calculated. You can exploit this to run the different operations with different tools (say a 1/2" end mill for roughing, a 1/4 ball mill for finishng and a 1/4 endmill for the pencil finish): save each operation as a different file and as long as you don't mess up the machine zero when you change tools you can run the files sequentially.

The spindle speed is not controlled my Mach3. It runs at 10,500 RPM but can be dialed back to 1100 with different pulley settings. See page 55 of the green binder and please leave a note on the machine if you change it.

Other possible "Gotchas" in this program. In the toolpath generation make sure you click the "Use Inch" button bottom right. And when you save the file make sure that the file type is Mach3-Inch(*.nc). Deviations from this may screw up your size by about 25x!

Once you have the .NC file, you can open Mach3Mill. Before you do this, make sure that the mill (especially the spindle switch and the spindle controller in the 6" black box on top) are all off. Once Mach3Mill is running you can turn on the main controller, the spindle controller, and the spindle switch. If you load Mach3 with the spindle switch on it can start the spindle which might not be a good thing depending on where your fingers are!). Once Mach3 is running, turn on all 3 switches.

From here, the instructions in the green binder, starting on page 10, can pretty much be followed. If they are TL/DR here is the brief version. Switch to the ToolPath screen (3rd from left) and click the reset button.

The keypad up and down arrows jog Y, left and right jog X, PgUp and PgDn jog Z. You can move the table around at will. The jog rate % will speed or slow this movement.

End Stops are a pain. Sometimes when you hit one you can reset and jog away from it (may take a few tries). If that doesn't work you have to drop power to the motors (turn off the controller) and manually turn the lead screws. For X and Y I cut screwdriver slots into the ends to help with this.

Secure your piece. Depending on what you are doing, a sheet of 1/4 hardboard under the piece will save the mounting plate. I have another at home that is chewed up if you have a task where adding a spacer is not possible.

Install your tool. I have left a few mills with the machine. If a tool is there, go ahead and use it. Moving forward if the space needs more variety it will need to be discussed. Note, the mills are held in a collet. When you change collets the nut that holds them seems "wrong." It is intentionally offset. See page 59 or the green binder or check with someone who knows how to do this.

Mach3 should start with X, Y, and Z  somewhere in a reasonable range. In the screencapture they are all +1.0000. Assuming you have the table roughly centered, you should set these if they are unreasonably large. I.e. if Mach3 was previously closed with a file that was fouled up beyond all recognition Mach3 might start thinking it has X at -280 or Y at +5500. You can click in the box, type a number, then hit enter. We will reset all these in a minute, but getting them close avoids a problem I have had loding the file. Which is what we'll do next:

Click the Load G-Code button and find your file (the first roughing cut file if you saved multiple paths). Once it loads, check the program limits panel at the top right of the screen. This should pretty closely match the size of your piece. If you are ~25x off, you have a mm to inch conversion error somewhere. Note the comment about Fusion 360 writing Mach3 files at the start!

Back in MeshCam you picked an origin. So next you need to get the tool centered on that origin as closely as you think you need. If you have plenty f stock, you can get X and Y "just close" but you will want to get Z as close to zero as possible. Use the jog keys to bring the tip of the bit to whichever part of the stock you chose as the zero. When you get somewhat close slow down the jog rate and sneak up on it. Once you have the tool set at what you think is 0, 0, 0, set the X, Y, and Z positions to 0, 0, 0. (When I was trying to get front and back register in jewelry waxes I would set X and Y using a tapered mill that came to a sharp point and viewed through a 20x loupe, zero those axes, change to the actual cutting tool and then zero Z.

I always do an air cut. To do this the goal is to fake where Z is so that the machine follows its cut path in the air above the piece. So if the full depth of the Z cut is 0.5 inches I would want to pretend that the Z zero is at least an inch above the piece. You can jog Z to +1, but it's easier to get it exact by putting a command in the MDI line. Click in that box and type G0Z1 (that's G zero Z one). The machine will move to Z = 1. Reset the Z coordinate to zero in the Z window at the top and you can then click Cycle Start (you can leave the spindle on or turn it off with the switch before you start).

You have a pink crosshair that shows where X and Y are. Blue lines to show where the toolpath goes, which turns to yellow after the path has traversed that point. A down arrow on the right shows Z movement and the G-code in the top left window will scroll as the lines are executed. I usually watch just enough to convince myself that the ranges look good and then hit stop. This will leave the mill at some random position. X and Y will be the correct positions and Z will be relative to the fake 1" above true zero we set earlier. So, in the MDI window type G0Z0. This will rehome Z to the fake zero point which is 1 inch above the true zero. You can then reset the Z coordinate at the top to +1. If you want to you can re-zero X and Y by typing G0X0 and G0Y0 in the MDI window but it's not really necessary.

Click rewind (to go back to the start), make sure the spindle controller is turned on, put on safety glasses, click Cycle Start.

Occasionally when you start the spindle will draw too much power (I think) and the machine will emergency stop. As long as the axes still know where they are you can just hit reset, rewind, and start again.

If you try to machine multiple toolpaths with different tools, you need to make sure that you leave some of your original Z=0 stock to be able to zero the Z axis with the new tool installed. You can move X and Y wherever you want to do this between runs.

When the run finishes, make sure Z is well clear of the piece (jog or MDI G0Z2) and then get the spindle out of your way (jog or G0X4 or so) and turn off the spindle control before you go poking around with fingers and wrenches. That's about it.

MeshCAM seems good with .stl files as long as the units are OK. I have created stuff in Blender (not an expert) and Rhino (ditto) that has worked out fine. I have also used BobCAD (no relation). The machine came with a license and a lot of my jewelry was created using this software. I think it is a fairly powerful system. Unfortunately my brain doesn't seem to "get it" and I found that whenever I left it for a few weeks I needed to pretty much relearn it. But there is a legal copy of V25 on the computer, plenty of online tutorials, and a set of traing CDs if anyone is interested. It will generate a toolpath for the mill (see the green binder) and it will also read stl files (although not from all sources; some header issue I imagine). The computer isn't quite up to spec but it seems to run, and if we have any compatible memory kicking around I think it will improve the performance.

Please fill all the letters into the box to prove you're human. V C R C I Please keep this field empty:

Edit summary

Note: By editing this page you agree to license your content under the following license: CC Attribution-Noncommercial-Share Alike 3.0 Unported

Asheville Makers Wiki

Site Tools

Page Tools