First steps with a Shapeoko router table

I ordered a couple of Trend router collet reducing sleeves - one reduces the 8mmØ DeWalt collet to 6mm capacity, the other does the same from ¼ inch to 4mm. These will allow the use of the smaller metric cutters without the excessive overhang imparted by the ER11 collet chuck. They arrived today and look to be well made but, by golly, they were expensive. One cost an arm, the other, a leg. (Actually £30 the two, delivered.)

Just tried out the 4mm ball end mill in the sleeve and, after re-zeroing the Z-axis, it appears to cut correctly. I must have failed to re-zero properly when I did it in the last video, having checked and re-checked the Gcode a number of times in Fusion 360.

I'm going to rotate the workpiece in the vice 180° and have another go at the entire milling procedure tomorrow. If that goes OK, I might have another attempt at aluminium, though at much reduced depths of cut, around 0.4mm, as suggested by Jason.

I've also found a piece of aluminium round stock sufficiently large to make a reducing sleeve for the router clamp, so that I can mount the ER11 spindle motor, currently set up as a tool post cutter/grinder attachment, directly in the Z-axis, to see how that will go. It's an air-cooled one, not the water-cooled version that would be preferable.

John

Edited By John Hinkley on 27/05/2021 16:22:27

Edited By John Hinkley on 27/05/2021 16:22:53

Well done John following this with great interest.

Now that it is tomorrow, I've revisited the conrod machining and - surprise, surprise - it didn't turn out half bad, even if I say so myself. Still got to make a few tweaks to a ramp height, but nothing too drastic and I'm getting all fired up for another aluminium session. First, though, I'll make a fixture to hold it securely in the vice and I think I'll add some tabs to stabilise it so thatwhen it's flipped to do the second side, it won't be cut out completely and risk catching on the cutter.

Latest video here:

You're getting there.

I might be tempted to reduce the plunge rate a bit particularly when you get to the alumminium so the tool does not drop down into the cut quite so fast.

The other alternative is to have it ramp down into the contour which also eliminates the need for it to lift and plunge each time it cuts a new layer. You can do this in the linking tab (yellow one) by ticking ramp. The only thing to watch is that if you only tick ramp at the end of teh cut it will lead out away from the finished edge into solid material so you need to set leadout angle to zero rather than 90deg, see below

Thanks, Jason. I think that I’ll try out those settings and re-run the code in thin air but with the cutters mounted, just to see the effects. It was my intention to reduce the plunge rates in addition to the depths of cut before taking on the aluminium again.

John

If you do try it then set the Max Ramp Step to the max DOC you want to use eg 0.4mm not the 16mm in the image above. You can have a look at the way it changes things on the F360 simulator and then see if the air cut is the same.

Thanks, again. Just tried that and somehow managed to lose the changed file. I hate the way Fusion stores everything in the clouds. I much prefer to have it on my computer but don't see how to do that.

John

You should be able to list all the revisions if you click the data panel and then the box with your conrod will have the latest revision number with an arrow next to it, click that and all the saved versions should come up. Hold the mouse over your name on the revision you want and click the file icon that comes up to open.

I see. I Googled it and it said to use the export option. So I tried that and it worked, so now I have two ways! London buses and all that!

John

Spent a bit of yesterday and some of today making a fixture to hold the aluminium stock for my attempt at milling the con rod shape. I half-inched an idea from Cough42 (he of electronic lead screw fame on YouTube) but modified it a little:

Here it is mounted in the vice. The bed of the router table is not necessarily exactly parallel to the plane of the X_Y axis carriages, so I've fitted some grub screws which bear on the top of the vice jaws that I hope will allow me to line up the top surface of the fixture using a dial gauge attached to the Z-axis carriage. That's the theory. Let's see if reality proves the theory correct. I'll make a video and that will show what happens. Three screws would have been better, of course, but there's nothing for the third one to bear on. The two dowels are silver steel rod pressed into the base at the centre distance of the little and big ends. This means I'll have to revert to material 10mm thick and do away with the facing process. As my stock of aluminium is severely depleted, I'm going to double- and triple-check the Gcode before committing to a full-blown run and publishing the results on here and YT.

John

That should read Clough42 for those doing a search!

Realised much too late to edit it!

John

Not done much for a couple of days due to family commitments, but finally got back into the workshop to do some more experimenting. Soon wished I hadn't. It did not go well - again! I should train myself to clear out all my old, unsuccessful gcode efforts from my computer, rather than keeping them in a random order of versions. Also, in an attempt to reduce material wastage, I altered the stock size for the various stages - or at least I though I had. Turned out the last stage (of course) was the one I hadn't and the router merrily chewed metal away from somewhere it shouldn't have done. Not only that but the whole outline shape seems to have altered. Goodness only knows how, but I'm going to have to go through all the processes again to try to find where I've gone wrong.

Here's the latest disaster movie:

Your getting there.

For the reduced thickness of the rod you could try reducing the stepover which may give a better finish and to avoid the tool cutting into the metal beyond the contour cut set the "tool center on boundry" or max 2mm offset from ctr that way the outer edge of the tool won't move so far sideways. It's the third box down on the geometry tab "tool containment"

For the 4mm ball nose set a smaller stepover much like your stepdown when contour cutting 0.4mm or so will do it in 5 passes rather than one.

The pocket being out of position looks like you may have zeroed the edge of the tool rather than allow for half radius or entered it as -2 rather than +2. Once I start cutting a part I keep X and Y at the same zero and only alter Z as I change tools due to their different lengths, the ctr of the tool does not change.

Not sure about the shift in length. Was the Big end OK or had that moved too? if so that would point to Y being a couple of mm out when locating the edge.

Jason,

I've had time overnight to mull over your suggestions and take another look at my drawings etc. I'll try experimenting with the changes in your first paragraph once I've got the unintentional offset sorted. I believe that it is a result of me changing too many variables at once, rather than taking a logical step-by-step approach. Firstly, my MDF cuts were based on stock material dimensions of 50mm x 120mm x 12mm. When I converted the files to suit the aluminium stock at 40mm x 105mm x 10mm (because that's what I had), I incorrectly altered the stock size in Fusion 360; in the case of the last relief pocket, it appears that I didn't change it at all, hence the wayward cut. Add to that another change to the position of the "big end" location dowel by 1.5mm and an inability to subtract one number from another correctly and I ended up with the machining all starting from a false offset. All in all, I couldn't have made a worse mess of it if had tried. But, hey, am I disheartened? You bet I am! Never mind as long as I have breath in my body and MDF in the workshop, I'll carry on until I get it right.

John

Despite my last comment above, I've decided to give it a rest. At least, for now. As you will gather from the video below, I'm pretty disheartened at the whole project. Not with the router - that's doing everything I tell it to do. It's just that I think I'm telling it to do the wrong thing, or rather the right thing from an incorrect starting point.

I believe that I have misunderstood from the get-go, the initial positioning of the milling cutter. I had assumed that the centre axis of the milling cutter should be directly over the origin of the "Work coordinate system", whereas by setting the cutter edges to just touch the stock in X and Y (i.e. 3mm off the origin), I would probably get the machining in the right place. Too late, I realised this and you will hear from the soundtrack that I'm a bit miffed and thus a break is called for.

I may try a bit of engraving, but no more milling. Others have made the machine work perfectly satisfactorily so it's definitely me, not the router. I just can't get on with the CAM.

Here's the video:

John

When I first started designing I found CAD to be very difficult. Now it is only quite difficult. I was 3-D printing and only had to enter the design into the slicer and then print. Then I set up my mini-mill with CNC and had to try to learn CAM. I found that to be even more confusing. To keep from wasting precious metal, I will take the extra time to mill the part from wood of which I have a lot, then when I feel the program is doing what I want, making cuts the depth I want, and where I want them, then I will switch to the metal for the actual part.