First steps with a Shapeoko router table

[John HinkleyParticipant @johnhinkley26699]

Duck, everybody! Watch out for all my toys coming out of the pram ……..

I tried the Shapeoko version of air-guitar and it seemed to work OK. The spindle – sans cutter and not running – moved from its zero position, appeared to do a helical cut downwards and proceeded to perform the pocket cutting manoeuvres. Great, I thought, I'll try it now with a cutter. I did, having set up the Z-axis to zero on the top of the workpiece. Switch on, run , set spindle motor running and press "go". Zoom, off goes the head and wang! straight down 10mm into the workpiece, then starts to try the helical cut. By this time my hand had reached the mains switch and I aborted the run. Another failure, more aluminium welded to the cutter and another hole in an otherwise useful bit of aluminium.

Somewhere along the line, I'm getting 10mm of unwanted downward motion and I can't for the life of me work out where its coming from. I strongly suspect I'm setting the tool heights wrongly in CAM section, but how, I know not. Don't bother looking for the video, I can't bring myself to string all these failures together.

I'm going to take a few days off to gather my thoughts and do a bit of gardening.

John

[John HinkleyParticipant @johnhinkley26699]

Well, I took a few days off to let my hair grow back and watch a few more videos. I revisited Fusion 360 and generated some new Gcode to attempt to produce a 2mm deep pocket in some MDF laminate flooring off-cuts. What happened is documented in this brief video:

Gives me a bit of renewed enthusiasm for further experimentation.

John

[JasonBModerator @jasonb]

That's looking better, good idea to just use something a bit more forgiving while you get the hang of getting your heights and positions right, when you can do that consistently then try some similar shapes in aluminium

[John PParticipant @johnp77052]

Hi ,
You could try this for test cuts ,re-melt into blocks or sheets for test cuts,
if the machine is clean catch the wax swarf and re-melt again to reuse.
No blunted or broken cutters.

MOULD CASTING WAX 2KG FOR LOST WAX INVESTMENT CASTING

from

https://www.artisanfoundry.co.uk

Similar to this prototyping wax.

John

[Michael GilliganParticipant @michaelgilligan61133]

One small step for Man … one giant leap

MichaelG.

[John HinkleyParticipant @johnhinkley26699]

Jason – yes, I’m going to try some more shapes and different cutting styles in the next few days.

John – that looks interesting, but I have a large supply of those mdf floor laminates to munch my way through, first.

Mike – I’ve heard an expression similar to that before, I think!

John

[John HinkleyParticipant @johnhinkley26699]

Just a quick update on the import duty/VAT situation. I've left it until now so as not to tempt fate ………..

I have received NO invoice from Fedex at the time of writing. I have contacted them twice asking for information on this specific delivery and all I got was a standard reply inviting me to open a Fedex account, which I have declined – I have no use for one. So, either I've "got away with it" or I can expect the bailiffs to be knocking on the door anytime soon, demanding wads of cash.

John

[John HinkleyParticipant @johnhinkley26699]

Risking boring you all with my failure to get to grips with Fusion and the router, I've just posted this video on YouTube. It represents an improvement, of sorts, in my understanding and implementation of the CAM function in Fusion 360. The first three processes went OK, but when I stopped to change the cutter and then reset the Z-axis zero accordingly, it went downhill, extremely rapidly. At about 1220 mm/sec actually. What performed perfectly within Fusion in simulation mode, suddenly drove itself into the work by an extra 5mm or so. I've checked the code for depth errors and everything looks OK. I think I'll try to get some reducing sleeves to fit the 4mm and 6mm end mill cutters into the DeWalt 8mm collet, to reduce the loss of headroom when using the ER11 chuck.

Let me know if you want the pain to stop and I'll finish the thread here – at least until I have something really positive to post.

John

[John HinkleyParticipant @johnhinkley26699]

Any significance in the timing of the above posting, do you think?

John

Pure coincidence, by the way. I didn't do it on purpose .

[JasonBModerator @jasonb]

Well at least the MDF is a bit more forgiving, I can't see anything obvious as to why it cut too deep. I assume you are touching off on the top of the stock each time and entering the Z height as Zero each time.

Luckily I did not have the video running yesterday on the conrod that I mucked up along with snapping the cutter, always seems to be the last stage that things go wrong, I can see what it did in Fusion and mush have been playing around with it between checking the simulation was OK and doing the post processing

[John HinkleyParticipant @johnhinkley26699]

That’s hard luck, Jason, but reassuring for me to know that more experienced people can have these issues too. And yes, I did touch off on the stock and re-zeroed the Z-axis after changing to the ball ended cutter. I have a couple of tweaks to try before attacking another piece of mdf.

John

[John HinkleyParticipant @johnhinkley26699]

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

[Graham TitmanParticipant @grahamtitman81812]

Well done John following this with great interest.

[John HinkleyParticipant @johnhinkley26699]

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:

John

[JasonBModerator @jasonb]

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

[John HinkleyParticipant @johnhinkley26699]

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

[JasonBModerator @jasonb]

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.

[John HinkleyParticipant @johnhinkley26699]

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

[JasonBModerator @jasonb]

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.

[John HinkleyParticipant @johnhinkley26699]

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

[John HinkleyParticipant @johnhinkley26699]

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

[John HinkleyParticipant @johnhinkley26699]

That should read Clough42 for those doing a search!

Realised much too late to edit it!

John

[John HinkleyParticipant @johnhinkley26699]

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:

I hope you are learning from my mistakes! Unlike me, it would appear. Perhaps I should go back to using mdf in the meantime.

John

[JasonBModerator @jasonb]

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.

[John HinkleyParticipant @johnhinkley26699]

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

[Author]

Posts