First steps with a Shapeoko router table

[John HinkleyParticipant @johnhinkley26699]

Contrary to what I wrote above, I've run the test piece of Gcode from the manufacturers and here's the result:

Hope that works.

John

[Michael GilliganParticipant @michaelgilligan61133]

… Brought back fond memories of the Roland DXY plotter

MichaelG.

[John HinkleyParticipant @johnhinkley26699]

I've spent 4 days or more trying to learn Fusion 360 – specifically the 'Manufacture' section in order to produce some workable Gcode for the Shapeoko and I think I've done it – at least I've got some that gives a result.

First real-world project was to produce a sacrificial wasteboard to protect the supplied baseboard. I used MDF as intimated above to make a board which not only protects the baseboard but had a matrix of mounting holes at 50mm centres fitted with 6mm screw inserts which can be used for securing workpieces or workholding devices to the machine. Originally, the board was to be populated by 50 inserts – so that's what I ordered. As the design evolved the number grew and now it's a matrix of 81 holes (9 x 9) at 40mm spacing. So that's a further wait until the second batch arrives. Should've ordered 100 in the first place, but too tight!

Published another short video to show it in action:

In the first section, I was using a 2-flute 6mm end mill to make the securing holes. Much heat was produced with attendant smoke but fortunately no fire. A short breather for a re-think and drills were substituted for the subsequent operations.

I think this will be the last posting in this thread until I have some decent footage 'in the can'.

John

[John HinkleyParticipant @johnhinkley26699]

Well, folks, things have moved on and sideways! I've been thrashing about with Fusion 360 trying to produce some Gcode for the router. The results seem to work OK in simulation so I tried something a bit (too) ambitious – cutting some aluminium. Sent off for some brand new carbide cutters ready for the onslaught and finished the wasteboard attachment. Buoyed up with my success with that, I looked forward to churning out lots of bits of CNC'd stuff. Oh, if only it was that simple!

First, I had to devise a means of securing the workpiece to the machine, so I dug out the set of low-profile clamps that I made for the mill. The attachment holes needed sleeving down to fit, so there's another delay. That done, I held the workpiece on both sides, not realising that the forces involved would be sufficient to dislodge it. Watch the video to see what happened. Suffice to say, it's time to stop, take stock and start again.

I'm going to re-align the workpiece with the router table, using a dial gauge or DTI and maybe put the vice from the shaper on temporarily to hold it, rather than using the clamps. I'll post a further report later, if there's still interest.

John

[Michael GilliganParticipant @michaelgilligan61133]

Thanks for sharing that ‘warts & all’ John

I’m sure it will set some sensible expectations.

MichaelG.

[JasonBModerator @jasonb]

John my thoughts.

1st attempt way too much depth of cut for that machine particularly as using the full cutter width.

2nd attempt still too much depth of cut for this machine and far too slow a feed rate given the rpm. I'd also suggest rather than contour you think about doing some adaptive cuts first and then just very fine contour passes to finish both using a lot more of the side of the tool not just the end.

Looking at Creative3D video for a contour they suggest 16Krpm, 800mm/min feed for your 2 flute cutter, 0.4mm DOC.

For Adaptive, 16Krpm, 1600mm/min feed, 1.9mm DOC x 0.6mm stepover

[John HinkleyParticipant @johnhinkley26699]

Jason, that's just the sort of insight I need to make progress. I did slow the feed rate to 720mm/m but the depth of cut was obviously too much. Perhaps I should keep my experimenting under wraps until I get better results. But then no one would avoid the pitfalls I encountered on the way.

John

[JasonBModerator @jasonb]

That second attempt looks a lot slower than 720mm/min, I count about six seconds to do a cut 25mm (4 x diameter) long so that's 250mm/min. Compare it with the first adaptive cuts on this part where I'm moving at 500mm/min

Edited By JasonB on 05/05/2021 15:55:48

[John HinkleyParticipant @johnhinkley26699]

Right again, Jason. I actually reduced the feed rate to 200 mm/m to try to replicate a similar speed to what I would have used when machining manually. And guessed the figure at that. I'm going to start over with a new piece of stock, held differently to ensure repeatability and accuracy.

I think I'l try holding a DTI with an 8mm mount in the DeWalt collet to check alignment.

John

[JasonBModerator @jasonb]

John, although you may feed at 200mm on the manual machine your spindle is going so much faster on the router and a slow feed will result in the tool rubbing and not cutting well.

Fitting the vice should hold the part a lot better

[Michael GilliganParticipant @michaelgilligan61133]

I wonder if it’s worth putting a speed-controller on that router

MichaelG.

[JasonBModerator @jasonb]

The downside to that is the feed will need reducing accordingly to keep the same low chipload and then the job starts to take a long time as the size of cut (width & height) can't really be increased due to the lack of rigidity.

When I worked it out in the other thread the Shapeoko should do a job on aluminium in a similar time to my KX3. It does that buy taking approx 3 times as many cuts in the same amount of time so if each of those cuts is 1/3rd of what I'm taking then total removal rates are similar.

The router is a vari speed one, not sure what John was adjusting it too but I would stick to No1 which is the minimum of 16K rpm and save the faster speeds upto 27K rpm for small cutters on wood etc.

[Michael GilliganParticipant @michaelgilligan61133]

Posted by JasonB on 05/05/2021 19:26:39:

[…]

The router is a vari speed one, not sure what John was adjusting it too but I would stick to No1 which is the minimum of 16K rpm and save the faster speeds upto 27K rpm for small cutters on wood etc.

.

I guessed so … but I was thinking of rather less than 16K [perhaps with the addition of a cooling fan]

I’m pondering what might be causing those burrs

MichaelG.

[John HinkleyParticipant @johnhinkley26699]

Fellas,

The quoted no-load speed range of the DeWalt 26200 router I have are 16,000 to 27,000 rpm so I was running it at about 20,000 rpm off load. I think I'm being a tad too timid in my approach to feed rate etc so I'm currently doing some re-jigging of the gcode to reflect the info Jason has suggested. The vice mount will have to wait until I've fabricated some new clamps – unless I can modify the shaper ones. I'll look tomorrow.

Thanks to all,

John

Corrected spelling!

Edited By John Hinkley on 05/05/2021 19:49:13

[JasonBModerator @jasonb]

 

Edit, posted before seeing Johns latest reply

Michael, I thought so as 16K is pushing it for a 6mm cutter but not sure if power would start to drop off if the speed came down too much. Two possible causes of burrs that spring to mind

1. No sign of burr at the beginning when it cuts across the corner before the work moved so could have damaged the cutter then

2. Looking again the router is set to speed No 3 say 22500rpm, combine that with a 200mm/min feed and a 2 flute cutter and that's a chipload of 0.004mm which is getting into the realms of rubbing, and not helped by dry cutting which may be welding metal to the cutter.

Edited By JasonB on 05/05/2021 19:50:59

[Neil WyattModerator @neilwyatt]

Posted by Michael Gilligan on 24/04/2021 14:16:35:

… Brought back fond memories of the Roland DXY plotter

MichaelG.

Reminded me of the Plotmate I used with my BBC micro. I once made a rough and ready double-sided PCB using it with an etch-resist pen.

Neil

[JasonBModerator @jasonb]

John, this is quite a good video that shows a couple of cutting options and talks about chip loads etc. and a good summary at the end. may be worth doing a few test slots like he shows in what is left of that workpiece before having another go at the conrod.

Michael, 25K rpm 2500mm/min feed of a single flute cutter and no burrs, does have a good grip of the workpiece though!

Edited By JasonB on 05/05/2021 20:25:09

[Michael GilliganParticipant @michaelgilligan61133]

Posted by JasonB on 05/05/2021 20:22:59:

[…]

Michael, 25K rpm 2500mm/min feed of a single flute cutter and no burrs, does have a good grip of the workpiece though!

.

.

I’ve only skimmed through it, but … That’s very impressive !

I note the heavy-duty fixturing, and the conspicuous absence of MDF

Sorry, John but I think you will need to be taking very light cuts, whatever the spindle speed.

MichaelG.

.

Just found this … in time for an edit:

https://www.ame.com/workholding-wisdom-posts/2021/03/10/the-role-of-stiffness-in-workholding/

Edited By Michael Gilligan on 05/05/2021 21:16:27

[John HinkleyParticipant @johnhinkley26699]

Me again, folks!

Having taken heed of Jason's wise words, I've relieved the shaper of its vice and mounted it on the router table. Fortunately only minor surgery to the bolt slots was required to align with the mounting holes in the wasteboard:

I also managed to mount a DTI directly in the router spindle in order to check the Y-axis tramming. The photo of the start, below, is taken from the video, so not very clear, I'm afraid.

Every journey has a start and an end and this is the end of that journey:

The DTI flattered to deceive as it remained solidly on the zero mark except for the last centimetre where it suddenly veered of by a miniscule* amount.

I'll publish a video later (probably tomorrow, now) and I think I'll gather them all together in a playlist as they seem, like Topsy, to just grow and grow in number.

John

*miniscule = a very small amount which I'm happy to live with.

[John HinkleyParticipant @johnhinkley26699]

I've taken a couple of days out to watch all the suggested videos and absorb as much of the advice as my poor old brain will take. Having reviewed the video that I took of the 2D pocket that I was trying out as a test, not only did the spindle veer off to the left of the stock, but impacted the cutter with such ferocity that it loosened it in the collet chuck. Upon closer inspection, it had also wiped both corners of the brand new carbide cutter. Out with the old and in with a new one. Back to the computer in the house and re-did the gcode with spindle speed 16,000 rpm, feed rate 1220mm/m and doc of 0.4mm. The simulated run in Fusion went well, so, with some trepidation, I ventured back out to the workshop and fired it up again. Set the camera rolling and pressed the 'go' button. Rapid movement to roughly the start position and wham! Down goes the spindle directly into the stock to a depth of 10mm and out the other side. Mad panic rush for the mains switch and peace is restored. I had to loosen the vice jaws to unlock the stock and spindle from their intimate grasp and inspect the cutter. Fortunately no damage had been sustained but aluminium had filled the flutes and welded itself to the cutter. Retired back inside to lick my wounds and have a cup of tea and a biscuit.

I have no idea what I'm doing wrong and, to be truthful, I'm getting more than a bit ticked off with it! I can only think that I'm setting some parameter or two (or more) wrong in the CAM section, somehow. But that doesn't explain why it works OK in simulation but goes seriously awry on the machine.

I think I'll have a go at wood next time, otherwise I'm going to run out of aluminium, none of which I would describe as scrap, or carbide cutters, or both.

My wife wants a new house number plaque, so maybe that might be a better proposition. I'm trying to run before I can even crawl, I think.

John

(Tail firmly between legs!)

 

Edited By John Hinkley on 09/05/2021 14:13:48

[JasonBModerator @jasonb]

Possibly the height you are setting the tool at relative to your datum point.

When doing the CAM setup you can position the 3 way arrow at various points on the stock. I usually use the top as it is then easy to use a block of known thickness ontop of the work to set the tool height. I use a 20mm block and enter my tool height Z as = 20 that way the machine knows my tool is 20mm above the top which is my zero.

If you have that 3 way arrow at the bottom of the stock you need to set your height from there.

[John HinkleyParticipant @johnhinkley26699]

Jason,

I believe that you may have hit the nail on the head. I have been setting the X-Y-Z position in Fusion to the south-west corner on the top of the stock and this results, as I say, in the simulation running OK. The clearance height is set to 10mm.

When I go to the Shapeoko, I have been setting the centre of the cutter to the south-west corner of the vice-mounted stock and then setting ALL the axes to zero. If I understand you correctly, I should be zeroing the X and Y axes to that position, but raising the Z axis by 10mm (the Clearance height) and then zeroing the Z axis? Is that correct?

I'll give it a go tomorrow to see what happens.

John

[JasonBModerator @jasonb]

No Stock top is Zero in that case, a clearance height of 10mm means the end of the tool will be 10mm above zero so clear the work by 10mm as it moves about from one position to another. If you are edge finding X & Y that is fine but what are you doing for Z? If touching off the top surface with a fag paper or similar then enter Zero. If you are using a block to gauge height which is safer than jogging the tool down too far then enter the height of your block as the Z value

Try a few air cuts with the height set well above the vice/stock and check all is well first until you track down the problem.

[John HinkleyParticipant @johnhinkley26699]

Damn! I am using the fag paper method of finding the zero position and setting Z axis to zero there. I'll abandon my last suggestion, therefore. I will set it as you say, then remove the ER11 collet chuck and cutter and try your air cut method. I should have plenty of airspace to play with that way.

Thanks for your patience,

John

[BazyleParticipant @bazyle]

I'd suggest first run with piece of balsa wood shaped like a cutter, cruicially same length protruding, and no stock or vice even in case the head whacks that. Then after two runs to double check move to cheap cutter and machinists wax or expanded polystyrene material.

[Author]

Posts