Bed for 6040 CNC?

[JasonBModerator @jasonb]

Probably get away with 16mm unless you are the very heavy handed type.

[Steve355Participant @steve355]

Too late, I’ve ordered 25mm. The existing flimsy bed is 20mm so I’m barely losing any Z. And it wasn’t much more expensive.

And I think rigidity increases with the cube of the thickness or something so it’s probably worth it.

Now though I will need to mill a bunch of M8 holes though 25 mm of aluminium, so I’ll need an appropriate cutter for that (?) . Alternatively use the CNC to mark starter holes and do it on my pillar drill.

[Steve355]

On Steve355 Said:

Now though I will need to mill a bunch of M8 holes though 25 mm of aluminium, so I’ll need an appropriate cutter for that (?) . Alternatively use the CNC to mark starter holes and do it on my pillar drill.

Drill them with the CNC…

I used M6 on a 38 x 38 matrix (as a compromise between the number of holes, something that would cover most of the available travel and avoiding various existing fasteners). I think I used 5000RPM for the drilling the 5mm holes, which is on the fast side, but it worked.

I spot-drilled first, then drilled through, then chamfered the tops of the holes. I tapped them by hand which seemed to take ages – might want to look at thread milling them on the CNC, especially if you stick with 25mm spacing.

Some rough video:

Spot drilling

Drilling

Chamfering

(I had to reduce the toolpath radius in the chamfering op as I ran out of machine travel. It looks like the tool is just plunging, but it is, in fact, circling around the top of the hole.)

 

[JasonBModerator @jasonb]

If your spindle is too fast for a 6.7mm drill then as I said bore with teh mill, a 5 or 6mm dia carbide cutter going down in a helical path will allow the spindle to be run faster than a HSS drill.

Thread milling to less than full height will stop the risk of screwing anything in too far and jacking the plate off the bottom, much like a thread stops in a tee nut for the same reason.

[Steve355Participant @steve355]

Thanks to everyone who posted drilling videos, or sent them to me.

My tooling plate has now arrived 😎

First job is to attach it to the frame, which is much easier said than done. As I see it I have two options.

1) use the existing flimsy bed as a template for new holes in the new plate. (hint – the existing bed is in 4 pieces which would need to be secured together very firmly. centre punch the holes and drill them on the pillar drill.)

2) use the CNC. Unbelievably, the spindle of the CNC will actually reach all of the holes at one end. I can locate a drill bit or slot drill in one of the existing holes, and then knowing the exact dimensions of the frame, I can just have the CNC drill the 8 x 5 mm holes for me.

Then I can turn the plate around, secure it to the frame, and run the program again. With luck (Famous Last Words) everything should be okay.

Any thoughts? Or better ideas?!

 

Steve

[JasonBModerator @jasonb]

let the CNC do it.

[Steve355Participant @steve355]

It was all going so well …..

I have attached the new bed, went pretty well. CNC drilled pilot holes and I finished them on the pillar drill – mainly because my 4mm end mill (for 5 mm holes) was only 11mm long and the plate is 25mm thick.

CNC chamfered the holes and the bed is now attached and I’ve levelled it to c. 0.001”.

I did the CAM program for the fixing holes. However, when I ran it it went very wrong. The end mill jammed and the shed lights flickered as the VFD did its best. Either I don’t have a suitable end mill, or there isn’t enough clearance to evacuate any chips 20 mm down. Or perhaps it’s cooling.

Hopefully I haven’t knackered the machine. It flexed a bit but it’s done that before and seemed ok.

Perhaps my best bet is to get the CNC to drill a bunch of say 8mm deep pilot holes and finish it off on the pillar drill.

[JasonBModerator @jasonb]

So you have opted for M6 fixings hence the mention of 5mm holes or are you going for M10 as you mention 8mm?

There is really no need to go to full depth if you are using M6, 2D would be more than adequate, even M10 you would only need go 20mm deep. the advantage of a blind hole is you won’t drive a stud or screw too deep and jack the plate up off the bed.

A good air blast will help get the swarf out the hole, if you can pump cutting fluid into the flow even better as that will help stop material sticking to the tool, look at “fog Busters” Slowing things down will also give the swarf a chance to get out the way. Uncoated cutter specifically for aluminium with more helix angle will also help.

And don’t forget that when using a milling cutter to bore at just over it’s diameter the feed rate is far greater as you G-code is based on the axis of the tool not what the edge of it is doing.

[Steve355Participant @steve355]

Hi Jason

The fixing holes from the bed to the frame of the machine are M5 and I used a 4mm end mill to create 5mm clearance holes for that

The fixing holes in the plate are M8 so I’m milling 6.8mm holes for these. I was thinking to go all the way through so as not to create a bunch of swarf collectors on the plate but as you say, that’s not essential and it’s far easier if I don’t do that. I can easily mill 10mm deep holes.

At this time, there isn’t going to be any fluid cooling, because it is on a wooden base in the shed over the lawnmower. I will see how I get on with the tasks I am using it for, and decided that is necessary at a future time.

[JasonBModerator @jasonb]

You don’t really need a lot with the fog busters, 10-25mls per hours running will all stick to the swarf. Have a look at This thread on MEM

What you have squirted at that one hole will be more than that over an hours use.

[Steve355Participant @steve355]

Thanks Jason, I will take a look

 

Holes all milled now to 10mm, I think in the morning I will extend to 20mm using a hand drill, tap, then use the CNC to chamfer.

Then the really exciting bit which is peeling the blue plastic off.

 

[Steve355]

On Steve355 Said:

Either I don’t have a suitable end mill, or there isn’t enough clearance to evacuate any chips 20 mm down. Or perhaps it’s cooling.

 

You need to get the chips away from the cutter. A small jet of compressed air helps enormously – 3 or 4 PSI is enough. (The brass tube in the photo.)

I use a small amount of isopropyl alcohol (IPA) entrained in the air stream as a lubricant for aluminium as it dries to nothing (be aware of the potential fire risk though).

[Steve355Participant @steve355]

I think in my case, I was trying to use a 6 mm end mill a 6.8 mm hole, 20 mm deep..

I think whatever you do, The chances of being able to expel chips at the bottom of the hole are low. When I tried it with a 4 mm end mill, the chips sprayed All over the place, and the hole  was pretty clean when finished.

I actually have a vacuum attachment, which I wasn’t using at the time, which may have helped, I could purpose it as a blowing attachment.

however, feeding it with IPA like that, I think it’s the same mechanism of operation as the MOAB/massive ordinance air blast/mother of all bombs. I quite like my Shed!

[Steve355]

On Steve355 Said:

…feeding it with IPA like that, I think it’s the same mechanism of operation as the MOAB/massive ordinance air blast/mother of all bombs. I quite like my Shed!

Ha ha 😀

Not quite that bad – it’s literally only a drop every second or so, but you are right to be concerned.

[Steve355Participant @steve355]

A 50l tank of hydrocarbons is literally enough to blow you from Lands End to John o Groats if the mixture is right … 💥

Anyway, I’ve done it, drilled, tapped, chamfered. Overall it seems pretty good

 

my only concern is that the threads, which were tapped using a drill, may not necessarily be straight. I was really hoping to use these as reference points. Looks like I’ll have to do some experiments with a DTI to see how much I can rely on it. I expect that’s why thread milling is a good idea. But I don’t have the knowhow for that.

 

[JasonBModerator @jasonb]

A few plain dowel pin holes would be better which I think I suggested earlier, you need a bit of wobble room for the thread if it is not to gall so there will be some minor movement.

Datron use IPA on their machines to good effect, probably have extraction on the cabinet, would only really need a vent as the compressed air going in would carry any fumes with it as it vents out.

Don’t know what CAM you use but thread milling is fairly easy with F360

Edit, just had a thought if you make your pins with a slack thread an dunder cut it to join a short 45deg chamfer then they should find their position against the milled chamfer in the plate and pull themselves true. Bit like the bolts that hold the wheel onto your car, the holes are slack but the chamfers pull the wheel into position.

[Andy_GParticipant @andy_g]

You could machine a shallow counterbore in some/all of the holes to take a hollow dowel that’s secured with a screw through the middle into the remaining threads.

No matter how you cut the threads they won’t provide accurate location on their own – it always needs another feature.

[Steve355Participant @steve355]

I see, well you live and learn I suppose.

I think I like the idea of adding some locator pin holes. I think Jason probably did tell me that and I probably didn’t listen.

Any thoughts on diameter of pin/depth of holes/clearance?

[Steve355]

On Steve355 Said:

Any thoughts on diameter of pin/depth of holes/clearance?

I’d guess about 10mm diameter – see if you can find a convenient source of hollow dowels and counterbore the holes to suit (maybe bearing races or something). I would guess 1-1.5mm would be deep enough to locate them positively.

The beauty of CNC is that you can start with an undersize hole and gradually machine it bigger until you get the fit you want with the dowel, then machine the rest of them to that size.

[JasonBModerator @jasonb]

I’d be looking at at least 1 x diameter depth to locate a push in pin, 6mm would probably do if they are just being used as stops to locate work rather than hold work against any cutting forces.

If you can CNC drill them to 5mm dia than use a 4mm cutter to bring them to size the flute length would allow you to go to 10mm deep. Buy some dowel pins or cut some silver steel and then use a test piece of aluminium to get your hole size right.

[Steve355Participant @steve355]

I was in fact hoping that I would be able to create a combined locating and workholding system.

Apart from creating a more stable workholding platform with plenty of fixing options, which I think I’ve achieved, there’s a specific workholding problem I was hoping to solve.

I want to be able to longitudinally “v-carve” some brass bars. See below a pic of an example in wood. These will be generally 1”-ish wide, 1/2”ish deep and 9 1/2” long. (Note the pic shows a 1” thick 4 inch long bar which isn’t quite representative)

What I’d like to be able to do, is locate a bar against a few pins, tighten a few screws against it laterally, and run my carving program.

This means the CNC would have access to the entire top surface of the bar.

The carving will only be longitudinal , but it must be accurate to c. 1 thou and repeatable, and doesn’t require the bar indicating in every time.

The 9 1/2 “ length makes it unsuitable for most low profile vices i think, hence hoping I could design a system that would allow this to work.

Hence my threaded holes, which it looks won’t do the job.

[JasonBModerator @jasonb]

If you have a reasonable number to do then it is the sort of job that is worth making a jig for. Could be a piece of plate with two fixed bars, one drilled through the side several times for clamping screws. Some holes in the base plate will allow it to bolt to your newly tapped table.

Clock the undrilled side in true then locate it’s position and set Zero, locate the end stop and set the other zero. You can now happily drop your bits of brass into place and tighten the clamping screws while holding the brass against the end stop. Have the origin of the CAM files as the set face and stop and then you can just run the program, swap in a new bit of brass and so on.

Less job specific would be a flat bar that bolts to the table, have a horizontal hole in it for a stop pin and two or 3 home made low profile clamps to hold the work to the fixed bar. same clocking an dwork swapping method but it would be possible to use the bar and clamps in any position on the table for other job.

Hope those are clear, let me know if not.

Alternative is a two vice setup which is quite common.

[Steve355]

On Steve355 Said:

I was in fact hoping that I would be able to create a combined locating and workholding system.

 

This is the arrangement I was thinking of:

The ‘dowel’ has been increased to 13mm dia so that the M8 fastener head doesn’t overhang it.

Not sure that it would help with your specific situation though.

[Steve355Participant @steve355]

Project report… a bunch of dowel pins and lump of aluminium turned up yesterday for making a jig and creating some location positions on the table. So that will be the weekend’s project 🙂

The new bed I made has so far proved to be highly effective, I’m getting excellent finish on milled aluminium. It’s difficult to see from the picture below that the finish is good, but trust me there is very little or no chatter. So far my bed seems to be a good investment.

one thing I do need to work out, is how to paint aluminium to a professional standard. I have some etch primer and some spray paint which claims to be  “strong”. It’s not good enough so far.

 

 

[Michael GilliganParticipant @michaelgilligan61133]

Looking good, Steve

MichaelG.

[Author]

Posts