Buget Warco Major 5 axis conversion

[Robin Hewitt]

I have seen thinner ones, but when I saw your plate, I suddenly felt inadequate!. Do you think 25mm will flex?

Hi Mark

I don't know if mine is thick enough, won't find out until I run it in to an immovable object. (3Nm*pi)/0.005m pitch = 1885N driving force :whistling:

I'll do my best to answer your questions but I've only been doing this for about 20 years so I'm still learning.

does this mean I owe you a Hobgoblin?

Indubitably, if we ever meet I will expect beer

I have found some angular contact bearing that will fit, and they are rated at 14k rpm, dinamic load of 24Kn, do you think they would do the trick?

Probably be fine, you're going to find out for us. Probably when a fat tool gets lost in a lump of iron and starts trying to cut triangular shaped holes with a sort of hammer action. :naughty:

Last question, for the mo' , as you can see my finish on ally is poor, I have not yet aligned the column, but have read much which suggests that finish is related to vibration. I still get some vibration at alost all speeds, feels to me like column flex. Does your do it?, have you filled the column with Epoxy Granite or balanced you pulleys (mine has 2 inters .....pain)?

What's 2 inters mean?

Obviously you want to avoid vibration but cut quality depends on a lot of variables. I still get a crap finish at times so I have yet to sort it. My biggest problem is aluminium chattering when I change direction into a radius.

If I was asked to list the variables that result in a good finish in descending order of importance, I'd guess...

A machine that is much too big for the job in hand.
Minimise overhangs.
The right tool for the job.
The right lube
The right feed rate and rpm
Cutting downhill

My mill is somewhat different to yours. I have a cast iron box section plinth at the back below the round column, often as not the head is wound down until it rests on the plinth. If I lean on the spindle nose I can bend it about a thou, maybe two if it isn't hard down. Perhaps they changed the design because it was too flexible?

Bestest

Robin

[Tweaky]

Hi Robin,
I'll try the bearings and let you know.

By "inters" I meant two intermediate pulleys, so four in all. Every other Warco Major I have seen, had one intermediate pulley.
From my perspective, it is just another component to add errors to the setup. I guess I could dump one pulley, and get longer belts.

Thanks for the short list, by overhangs, do you mean the machine itself, or mounting of the workpiece?

The right tool for the job.
The right lube
The right feed rate and rpm

These are things I know almost nothing about yet. My experience with machine tools is confined to 1 year spent at a broad base engineering school, as part of an electronic apprenticeship, and that was 32 years ago. I have read much over the last few years, but there is no knowledge like experience, so I Know very little at the mo'.

I did not notice the difference in your mill until I read your message. It does seem then that the column is the problem, that you can remove it from the equation by lowering the head to the support, it's case solved then.
I have had a few ideas for improving things here, one was to mill square a large cast-iron wieght, and then mount the column support onto it, with the column through it.
I have enquired about a solid steel column, which could be cut with a groove to locate it radially, a la' Arborga mills.
A square column is the ideal I guess, but not a good use of time for me (silk purse and sow's ear etc. ) better to buy another machine.
So maybe i will have to be satified with small cuts.....?

A Fursty Ferret is calling me, so time to go.

Many thanks

Mark

[Robin Hewitt]

Hi Mark

Overhangs are tool tip extension from the chuck, how far the chuck projects below the quill, distance you wind the quill down to make the cut, height of the workpiece above the bed.

Small cuts are not a problem for CNC once you have got past the teething troubles and trust your setup and G Code not to go hideously wrong. A large job may take hours but that's okay for a hobby machine which doesn't have production deadlines and can simply be left to get on with it. Trust is the key to that, when it stabs you in the back find out exactly what went wrong and fix it once.

You will "hog it out" as our American chums would say. Rapid removal of the excess material followed by fine finishing cuts. Only problem with that is chatter can leave vertical striations which echo in to the finishing cut. A speed change can help.

You have to experiment and find out what you can get away with on your machine, unfortunately there doesn't seem to be much rhyme or reason to it. You settle on a fine finishing cut, then one day it goes horribly wrong and ploughs in to the body of the work. An enormous cut that comes up with a fine finish and you wonder why you aren't cutting it all that way.

HSS tooling takes a sharper edge than carbide but doesn't last as long. If you want a fine finish don't fall in to the carbide trap. A centre cutting tool is a bad idea if you are trying to get a fine finish on a horizontal surface but is essential if you want to plunge.

Lubes. A bottle of Rocol RTD is a good start. A suds pump is better than a brush, especially if you want to run it unattended, but that probably precludes the milling vice because it will dump the run off on the floor. Incidentally, very tempting to buy an enormous milling vice but that's a big overhang. If using suds a wet and dry vacuum cleaner makes chip removal and clean down a doddle. I run the suds back in to the tank through a filter bag to protect the pump. Cast iron should be cut dry but I have recently had luck with paraffin as a lube, expect to find hard spots. Avoid cutting stainless, it is horrible.

Cutting downhill is a good idea unless you have backlash issues. If you cut an external counter-clockwise the tool will tend to bend in to the job, if you go clockwise it will shy away from it. The tool tip will always leave a line regardless, some people hone a tiny radius on the end to prevent that, I've never tried it, prefering to go full depth on the final pass. It all depends on what your machine will let you get away with.

I have probably rambled enough, but let's have one more... avoid tool changes unless you have a really sneaky method to reset the tool height with incredible precision.

Have fun

Robin

Edit: One more, cockpit checks. When you get in an aeroplane you go through a list, hatches and latches, tight and secure, brakes on, off, pressure exhausted etc. Before you set the milling job in motion have a check list. Particularly, are the chuck, drawbar and clamps on that round column stupidly tight. Do you have enough movement on the table to do the job? Will a G0 run the tool through a hold down fixture? The spanner Warco supply to clamp on to the round column isn't up to the job, suggest a socket or a box spanner, or extend the nuts so you can get a ring spanner on them. The Warco drawbar head is held on with a pin and is best replaced in toto.

[Tweaky]

Hi Robin,
Wow, that’s probably more useful information than I have gleaned from memory and reading. Thanks

The overhang scenario is obvious, now you have pointed it out. I had assumed that if the extensions were solidly mounted and flex free, they would become the mount rather than a pivot.
You will probably laugh, when I tell you, that all my parts have been made using a humungous 6” tilt & swivel vice, bought on the premise that mass and solidity were king! …. Clamps from now on.
This leaves me with two problems now, my trunion table with a rotary table on top 170mm min., and the column, as the head will be that much higher.
Incidentally, the head clamping is by 3 large nuts (& bolts) which I tighten with a large ring spanner, so much so in fact that the column is free of grease (copperslip)
and won’t fall or crank, until I wind it up!

I have a fairly extensive range and quantity of HSS cutters (all imp.) so I am happy they will be useful, although I guess I will need a Tool cutter/sharpener in the future.
Are indexable cutters a good idea, I was thinking of buying a face cutter?

I had intended to use Castrol Carecut as my lube, because the heinous stuff we used in the 70s gave me dermatitis, but I have no idea how good it is as a cutting fluid, yet!

Well, lots to be getting on with, Z axis next to make, and I’m looking forward to applying this new found knowledge.
I do not have an angle plate large enough to mount the Z axis bearing block to bore them, so I am going to use the vertical rotary table (truniun mount to be) and find out how solid it is as a mount.

Many thanks for your time and for sharing this knowledge.

Regards
Mark

[Robin Hewitt]

When designing the Z remember that you will want to hammer tooling out of the spindle taper.

You don't want to hammer against the Z screw so some way to release it is a good idea.

The quill lock is probably not enough because you will want to draw them in tight. I use a sledge hammer with a broken haft because it fetches them with one blow.

A release also lets you use the machine as a drill without writing G code, which is totally handy.

Robin

Edit: I don't use indexable tooling and I have never thought about resharpening cutters.
Face cutting accuracy and finish depends on how square the spindle is to the bed. Inaccuracies becoming more pronounced as the radius of the cutter increases.

[irving2008]

So how do you do it Robin, I looked at the pics of your current Z and your previous Z I now have and i dont see how it is released?

[Robin Hewitt]

So how do you do it Robin, I looked at the pics of your current Z and your previous Z I now have and i dont see how it is released?

The enclosure around the Z screw nut extends down to the honking plate and bolts on from below. To release it I remove the bolts.

The snag is the screw wants to be as close in to the quill as possible but the tin housing at the top of the machine overhangs, limiting the vertical space. I didn't want the screw to extend below the honking plate.

On the Mk 1 I had one 8mm bolt in the hole where the depth stop used to go. On the Mk 2, I used two 8mm bolts so I could extend the screw down to the bottom of the honking plate, passing between them.

It is a weak point because on the Mk 2 I cut threads in aluminium rather than steel which will wear and, eventually, strip. Hopefully I have cut them deep enough to see me out, one of the advantages of getting old :naughty:

[irving2008]

So you remove the bolts for every tool change? i can see why you'd want to minimise tool changes then!

[Robin Hewitt]

So you remove the bolts for every tool change? i can see why you'd want to minimise tool changes then!

I remove the bolts if I want to change chuck, not tool. Swapping a collet doesn't involve hammering. Changing from collet to drill chuck does, but I want to free it anyway if I'm going to drill.

Setting up a CNC mill is not what you could call 'a quick job' by any stretch of the imagination, bunging in a couple of bolts is not a big factor.

I have my own method, it goes something like this...


Glue a laser printed paper template to the workpiece using Pritt.
Saw off as much excess material as possible.
Drill mounting holes, using the template and the .dxf file that created the G code to get the X,Y right.
Remove all clamping and clean the machine down.
Change drill chuck for a collet chuck and fit a centre drill.
Drop the milling head down and lock it.
Bolt stand-offs to the table locating them with the centre drill.
Bolt the job to the precisely located stand-offs thus aligning it with where the mill thinks it is.
Drill a pip somewhere to get an alignment point I can refer back to if everything goes tits up.
Change the centre drill for a milling cutter.
Bolt the nut to the honking plate.
Move to a location that will be cut away.
Drop the cutter until it cuts through the paper.
Zero the Z axis.
Withdraw the tool and move closer to the start point.
Blow the suds return channels clear with the airline. (Best done dry).
Make sure everything is tight.
Get the suds in the right place, set the flow somewhere between "No flow" and "Splashing everywhere"
Main motor on.
Move to the computer and click on "Cut" then quickly move the mouse over the "Pause button".
Stand there, finger poised, until confidence wells up inside.
After about 30 seconds the suds has destroyed the Pritt so I can flick the paper template out.
Make tea, find cigarettes.


Edit: Forgot the splashguards, I use sheets of acrylic in the front and rear T slots. Probably forgot lots of other stuff but hey :whistling:

[irving2008]

I see.... well I am learning something here too...

I have a set of MT3 collets rather than a collet chuck. I can see a collet chuck would be easier to switch tools with and could help avoid moving the head up n down. Have you used the collet chuck for drilling, and if not, why not? My 16mm drill chuck is huge.. I am thinking of getting a 10mm one to be of a similar size (vertically) to the boring head so avoiding head movements when switching between them. But of course you wouldnt use a boring head on CNC, you'd use a small mill on a circular cutting path instead, although deep bores might be tricky.

What happens if the part has no through holes to bolt it down with, or are these in the excess? Presumably the reason for the standoffs is to allow you to machine around the outside and inside in one operation (and to space it off the bed? - or do you use a sacrificial?)