Bed for 6040 CNC?

[mgnbukParticipant @mgnbuk]

One of the companies I worked for tried building a machine tool from “epoxy granite”. There were a number of small trial parts made to prove out some aspects of the deisgn – basically using filtered coolant as a hydraulic medium for hydrostatic slideway bearings on as-cast epoxy granite slideways. As the moving element would not be in dierect contact with the slideway, wear would not have been an issue. One goal was to try to do away with traditional fitting (my MD at the time had an intense dislike of fitters ! ) by casting the finished product such that the machine “just” needed assembling.

One of the test pieces was a floating member, with pockets cast on the underside & pipes to the pockets cast into the block. The block was cast from varying sizes of aggregate mixed with a low viscosity epoxy resin ( Ciba Geigy IIRC – came in 2 x 205 litre drums). The working sruface was cast against a surface plate coated with release agent and, when tested showed that the hydrostatic idea worked in practice. The part was then (rather carelessly) put to one side such that it sat at an angle on two edges with the middle unsupported. I came back into the works after a period of working away and the Technical Director was keen to show how the project was progressing & placed the flaoting block on the surface plate to demonstrate it, only to find the tha block was nolonger flat. Despite an extended curing time, the block was not stable & would move over time if not fully supported.

The project did to proceed to building a full size machine, but by that time the hydrostatic bearing slideways had given way to convention linear guides. The basic outline of the machine was a sheet steel fabrication, with machined sections placed to have the linear guides bolted on & then infilled with a variety of concrete building blocks & varying sized aggregates bound with the epoxy resin, mixed in a small concrete mixer. The TD oculd be a bit incautious & did not take adequate care when working with the larger quantities of epoxy (the machine was a 1500 mm table diameter vertical borer, so the base “casting” was large). He ended up with severe skin problems due to contact with the resin that took weeks of application of special cremes under stockinette sleeves on his arms & hands to clear up the extreme reaction & was he subsequently so senstive to the epoxy that he only had to walk through a room where it was being mixed for the symptoms to flare up again.

Ultimately the project failed – one issue being the inability to work on the finished “casting” – as a developement project there was often a need to add something or other & it proved impossible to drill the material – HSS drills went through the steel shell OK, but dulled as soon as they hit the resin bound aggregate.   Hammer bits would not work on the resin/aggregate core, as the resin damped out the hammer action. Not possible to weld to the shell after it had been infilled either, due to burning the epoxy. Eventually a machine was completed & sold to a customer, but it proved so poor in service that it was bought back, stripped of useful parts & the “casting” had to be disposed of as controlled waste.

While composite construction may have advantages in some instances, I suspect there is a reason why cast iron is still the prefered medium for machine tool bases.

Nigel B.

[Steve355Participant @steve355]

That’s a really interesting story Nigel. Mine, of course is a home hobby machine on a much smaller scale, and very limited budget at this time, which is what might make something resin based seem like an attractive option.

Messing around with some engraving today I can see I will need a very flat, very level, vibration free bed…

 

 

[JasonBModerator @jasonb]

Unless you ar eengraving a 600x 400 sheet of metal it is usual to flaatten the area that the piece of metal is going to be fixed to before attaching it. For small items you can just hold a piece of MDF in a vice and level that. This was engraved and then drilled just using the tape & glue method to hold it down. I then used the screw holes to add additional clamping while I cut the outer profile. You can see level is reasonably good as I have cut through the part but not the masking tape below.

If a bit bigger then cut a piece of MDF just a bit larger than the item. This shows the heads of the fixings to the bed set below the top so you could again machine it flat first. Part was clamped to that MDF to drill the holes and then they were used for wood screws into the MDF to hold it for profiling.

If the part is reasonably thick compared to it’s thickness then it can be held directly in a vice, the top skimmed flat and then engraved

Your biggest problem is likely to be the lack of head room to get a decent size of vice into place but you should not need much Z axis height above the work for engraving and the cutters are short.

[Steve355Participant @steve355]

Jason – that’s very impressive. I have lots of questions about engraving! For a different thread.

“Unless you are engraving a 600×400 sheet of metal” – that’s the thing – that’s the plan really. Hence the CNC router rather than CNCing a smaller mill (e.g. my Dore Westbury).

Let me explain a little more about what I’m trying to achieve. My passion (no idea why) is those old woodworking moulding planes you find at car boot sales. I have made lots of them in my time.

 

Making the blades from O1 is a really miserable business. I’ve generally cut them out of sheets of O1 with my horizontal mill, but the skinny ones are particularly hard, and profiling the shapes on the end is time consuming. If I could cut them out with CNC I’d be 90% of the way there. Here are a few test cuts from hardboard.

 

I am aware that there’s potentially a speeds and feeds/lubrication/cooling issue here but that’ll have to be solved as and when I come to it. But that will likely mean that MDF is out as a base medium.

For my planes to be the coolest I want to make engraved brass end plates for them. See below an example in hardboard. You can imagine a sheet of brass being put in the CNC machine and off it goes creating a whole sheet of these while I do something productive.

So that’s the initial mission.  For the brass, that probably means a thick, skimmed piece of MDF. For the O1 it may mean a coolant tray and pump!

 

[Colin BarronParticipant @colinbarron94178]

There is a Boxford lathe base for £100 on facebook market place.

[Steve355Participant @steve355]

Well, some success to report even with no mods to the bed.

Cutting brass was a doddle. Engraving less so, all engraving bits I tried failed. I think I have the wrong type of engraving bit.

I expected cutting O1 to fail pretty much as soon as the cutter hit the metal. But in fact, it was generally fine. It was a 2mm 2 flute, running at 8000 rpm, 9 IPS, 0.005” DOC. it really liked a lot of cutting fluid, and I had to clean out the chips regularly. it didn’t quite bottom out, it needed another 5 thou or so. But light can be seen, so I judge it to be a success. it took about 20 minutes, which is a tiny fraction of the time  it was taking me before. I would really like to get the process so I don’t have to babysit it quite so much. I don’t know if that means flood coolant, but of course that would mean ditching the MDF.

There was some vibration, but nothing like as much as I expected.

But overall it is challenging me to consider what really is the best solution for a bed for this machine for these purposes . It’s possible that a thick piece of MDF, or chipboard kitchen worktop, well attached to the existing aluminium bed, might be the best way to go in the short term.

I do have other operations I want this machine to do though.

 

[JasonBModerator @jasonb]

The problem with cutting out contours with such a shallow depth is that you will quickly wear just the tip of the cutter. I would be tempted to try it a bit deeper at around 0.2 to 0.25mm

Is that the actual speed you used 9inch per second is extreamly fast or was it 9IPM? somewhere around 200mm/min (8ipm) is the right sort of ball park for such a small dia cutter.

If you have a compressor set that up with a fine nozzle to blow the swarf out of the way as recutting swarf soon blunts the cutter and can also make it deflect. Next up from that is to feed a small amount of cutting fluid into the air flow which lubricates the cutter, particularly good with aluminium but not so wet that your MDF will get soggy. Have a google for “fog buster”

You can see the small amount of liquid that is on the surface of the work, a lot less than flood cooling.

Brass can be done dry but the air will keep any pockets or slots clear of swarf

Post some details of what engraving cutters you were using as well as speeds, DOC and feed rate

[Steve355Participant @steve355]

Sorry, it was 9 IPM, not 9 IPS! Saying that I should basically double my DOC, fine by me, that will double the speed. I’ll give it a try.

I do have a compressor, but it’s unreasonably noisy. I think I need a quieter one. But, perhaps blowing away the swarf automatically with combined with manual oiling might work. I have a bad feeling that if I use a fine mist of cutting oil, my entire shed will end up covered in it.

On the engraving I don’t really know what I’m doing I’m afraid. I haven’t managed to find much decent advice online. The bits I’ve been using have been 15 degree. I have some 30 degree bits coming tomorrow. I think I ran them at 6ipm , 1400 rpm or thereabouts. The 15 degree bits were much too delicate.

One thing I do know is the text is small – typically 3mm high.

I am using the FreeCAD v-carve facility. I’m sure people will say “use X” or “use Y” but that probably isn’t practical as I have a huge amount of CAD modelling invested in FreeCAD.

Any advice on engraving would be very helpful.

 

[JasonBModerator @jasonb]

As the tip of any Vee shaped engraving tool is a very small diameter you want to be running at as high a speed possible, certainly in brass so your 1400rpm was far too slow. I’m limited to a 5000rpm spindle but would really like to run at closer to 20000rpm for engraving.

You also only have one cutting edge which means when working out the fee drate from the chip load and rpm your 6ipm was too fast for the slow spindle speed.

I’d be in the region of 0.01mm chip load so at 10,000rpm that would be 100/min or 4ipm. For 20,000rpm a feed of 200mm/min or 8ipm. Your 1400rpm would have worked out at 14mm/min or just over 1/2ipm.

This name plate is about 80mm long so same sort of font height as yours (2.5mm and 4mm) done with a 60deg 0.2mm tip cutter at 5000rpm and 50mm/min feed, depth 0.12mm. I design in Alibre and use the free Fusion360 CAM

 

[BazyleParticipant @bazyle]

One of your cut-outs in steel has a long straight edge. Why on earth would you not place that along one edge of the material to avoid having to cut it out slowly? Also just mark the other long straight line and hacksaw it.

[Bazyle]

On Bazyle Said:

One of your cut-outs in steel has a long straight edge. Why on earth would you not place that along one edge of the material to avoid having to cut it out slowly? Also just mark the other long straight line and hacksaw it.

Because this was a test of the capability of the machine and the set up. Indeed I would run it like you say. In fact, a “full set” of these blades has 32 similar cut-outs in it. They’d all be arranged to minimise waste.

I’ve cut many of these with a hacksaw and with a horizontal mill. It’s a miserable job. They also have to be very accurate. Doing it on CNC is going to be a blissful experience. Press the go button and have a cup of tea.

Actually that’s not the end of the story by any means. They also need tapering in thickness from 1/16” to 1/8” across the length. I usually do that on my old eagle surface grinder. That’s a boring job too.  I feel some CNC motors coming on for that, now I’ve basically worked out how to do CAD/CAM/CNC.

 

[JasonBModerator @jasonb]

Yes the earlier photos show some basic nesting of the three test pieces, and as you say you want to cut from large 600 x 400 sheets I would imagine there will only be a few near the edge and the other side of them won’t allow a hacksaw in due to the proximity of other blades.

A lot of CNC work you tend to start with slightly oversize stock and cut all round rather than have to faff about getting one edge spot on and if sheet it is unlikely to have a good machined edge to start with so needs milling anyway.

[Steve355]

On Steve355 Said:

That’s a really interesting story Nigel. Mine, of course is a home hobby machine on a much smaller scale, and very limited budget at this time, which is what might make something resin based seem like an attractive option.

Messing around with some engraving today I can see I will need a very flat, very level, vibration free bed…

 

 

On mgnbuk Said:

One of the companies I worked for tried building a machine tool from “epoxy granite”. There were a number of small trial parts made to prove out some aspects of the deisgn – basically using filtered coolant as a hydraulic medium for hydrostatic slideway bearings on as-cast epoxy granite slideways. As the moving element would not be in dierect contact with the slideway, wear would not have been an issue. One goal was to try to do away with traditional fitting (my MD at the time had an intense dislike of fitters ! ) by casting the finished product such that the machine “just” needed assembling.

One of the test pieces was a floating member, with pockets cast on the underside & pipes to the pockets cast into the block. The block was cast from varying sizes of aggregate mixed with a low viscosity epoxy resin ( Ciba Geigy IIRC – came in 2 x 205 litre drums). The working sruface was cast against a surface plate coated with release agent and, when tested showed that the hydrostatic idea worked in practice. The part was then (rather carelessly) put to one side such that it sat at an angle on two edges with the middle unsupported. I came back into the works after a period of working away and the Technical Director was keen to show how the project was progressing & placed the flaoting block on the surface plate to demonstrate it, only to find the tha block was nolonger flat. Despite an extended curing time, the block was not stable & would move over time if not fully supported.

The project did to proceed to building a full size machine, but by that time the hydrostatic bearing slideways had given way to convention linear guides. The basic outline of the machine was a sheet steel fabrication, with machined sections placed to have the linear guides bolted on & then infilled with a variety of concrete building blocks & varying sized aggregates bound with the epoxy resin, mixed in a small concrete mixer. The TD oculd be a bit incautious & did not take adequate care when working with the larger quantities of epoxy (the machine was a 1500 mm table diameter vertical borer, so the base “casting” was large). He ended up with severe skin problems due to contact with the resin that took weeks of application of special cremes under stockinette sleeves on his arms & hands to clear up the extreme reaction & was he subsequently so senstive to the epoxy that he only had to walk through a room where it was being mixed for the symptoms to flare up again.

Ultimately the project failed – one issue being the inability to work on the finished “casting” – as a developement project there was often a need to add something or other & it proved impossible to drill the material – HSS drills went through the steel shell OK, but dulled as soon as they hit the resin bound aggregate.   Hammer bits would not work on the resin/aggregate core, as the resin damped out the hammer action. Not possible to weld to the shell after it had been infilled either, due to burning the epoxy. Eventually a machine was completed & sold to a customer, but it proved so poor in service that it was bought back, stripped of useful parts & the “casting” had to be disposed of as controlled waste.

While composite construction may have advantages in some instances, I suspect there is a reason why cast iron is still the prefered medium for machine tool bases.

Nigel B.

I was chatting to my manager in 1980 who had worked for Alfred Herbert who told me that cast iron lathe beds were allowed to stand for months to stabilise the structure before machining.

[Steve355Participant @steve355]

Today I acquired a lump of 1” MDF from the local building suppliers scrap bin, and I’ve bolted it to the existing aluminium bed. This should create a much more rigid and damping surface than the flimsy bed on its own.

I have ordered a skimming bit, should arrive tomorrow, then I can flatten the MDF and I’m in a good position to have another go at the engraving, using suitable speeds etc.

[mgnbukParticipant @mgnbuk]

I was chatting to my manager in 1980 who had worked for Alfred Herbert who told me that cast iron lathe beds were allowed to stand for months to stabilise the structure before machining.

I did the last year of my apprenticeship at Boxfords (approx September 1980 – September 1981) at the original site in Wheatley, Halifax. At that time the bed castings for the “original” Southbend pattern lathes were matured outside for around 3 months before being shot blasted & having a rough cut planed from the top & bottom faces. The castings were then returned outside for another 3 months before coming in for another shot blasting, filling and painting & then finish machining. During the periods outside, the castings were watered down daily with a hose pipe if it was not raining or snowing.

During the time I was there the new geared head lathes were coming into production & one of the machines I worked with was the Snow bed grinder with Radyne induction hardening plant. The new bed castings were not “weathered” as they were supposed to have been heat treated by the foundry to remove the need. There were issues with the hardening process due to the partly machined bed castings moving during the induction hardeing phase. As there was only a small gap between the induction form (a hollow copper part, water cooled, that was the shape of the bed formation + the optimal clearance) any movement of the bed caused contact between the form & the bed, which resulted in a hole being blown in the form. Repair was time consuming & probably expensive. The cure was to modify the fixture holding the bed casting to take a substantial bolt about half way along the bed – a strap was used to pull the bed holllow before hardening & a torque setting for the bolt ( & thus the amount of defection) was found by trial & error that constrained the bed movement to prevent contact.  With the bed formation hardened, the strap was removed & the grinder table moved from the hardening plant end to the wheelhead working area & the hardened top surface of the bed was form ground at one setting. At the very far end of the table was a roll dressing attachement with a diamond coated roll that dressed the finished bed form onto the wheel.

I have some photos of the hardening process & a few shots around the Boxford works somewhere – I got a 35 mm Praktica camera for my 21st birthday around the time the Snow grinder was installed & expended an early roll of flim practicing using it. Not too many pictures though (and some not great pictures ! ) – buying & developing film took a chunk out of my not-that-generous apprentice pay packet ! I could hunt them out if there was any interest ?

Nigel B.

[Michael GilliganParticipant @michaelgilligan61133]

Always interested to know more about how things were done traditionally/properly, Nigel … in the days before the world went greedy and mad.

MichaelG.

[Colin Barron]

On Colin Barron Said:

…<br class=”bsp-quote-title” />I was chatting to my manager in 1980 who had worked for Alfred Herbert who told me that cast iron lathe beds were allowed to stand for months to stabilise the structure before machining.

Correct, but not a good thing!

It meant that a customer setting up a factory had to wait a year or two after ordering before his machines turned up!  The delay put a serious financial strain on new enterprises because a factory that’s not making product is burning money.   Machinists who don’t pay the bills may not mind waiting for a ‘quality’ machine, but investors can’t bear delays!

Things got downright nasty for many British machine tool manufacturers between the wars when customers realised they could buy machines with innovative automatic features off-the-shelf from abroad, notably the USA, but later Europe as well, and often at lower cost.  In part this was made possible by the development of Meehanite, a family of cast-iron alloys that stabilise quickly after cooling, and don’t have to be left standing for yonks.

In the UK too many conservative firms chose not to modernise their foundries, instead expecting customers to wait patiently for time to sort out their cheap cast-iron.   There was also an expectation that customers would pay well over the odds for hand-fitting and other ‘quality’ touches.   As a result customers walked away, and many British tool-makers suffered.

At the time it was claimed that foreign alternatives were of inferior quality, missing the point that forward looking customers wanted the latest and best in productivity, and only expected tools to last a decade or so.  For most of the 19th century low wages and absence of competition meant Victorians could profit from a high-grade manual machine that worked for 60 years plus.  Unfortunately, the 20th century changed the rules, and those who didn’t adapt died.

Herbert were more successful than most, but selling and making machine tools is brutally competitive!

Dave

 

[mgnbukParticipant @mgnbuk]

Herbert were more successful than most,

IIRC they effectively went bust in the mid ’70s & had to be bailed out by the Government to keep going, so maybe not that succesful given other competitors lasted longer.

At the time my late father worked for an office furniture company & one job he worked on at Herberts after the bailout was to install a new, bespoke, multi section rosewood finished table in the board room. At the time the directors still had their own, waitress service, dining room. Maybe if the Government bailout money had been spent modernising the business rather than on perks for the directors the company would have survived a bit longer ?

Nigel B.

 

[mgnbuk]

On mgnbuk Said:

Herbert were more successful than most,

IIRC they effectively went bust in the mid ’70s & had to be bailed out by the Government to keep going, so maybe not that succesful given other competitors lasted longer.

At the time my late father worked for an office furniture company & one job he worked on at Herberts after the bailout was to install a new, bespoke, multi section rosewood finished table in the board room. At the time the directors still had their own, waitress service, dining room. Maybe if the Government bailout money had been spent modernising the business rather than on perks for the directors the company would have survived a bit longer ?

Nigel B.

 

Another story from Herbert’s was a large lathe which was complete and about to be shipped to a customer and final inspection found what was maybe a crack.  The quality manager was summoned and no one could decide whether it was a crack or not.  After much debate and disagreement the QA manager sent for a mel hammer and smashed the lathe.  He said ‘there is a crack now’.

[Colin BarronParticipant @colinbarron94178]

When i was at poly, it would be about 1979, we went once a week with a fellow student to the staff canteen at Doxford Engines for our lunch.  The food was fantastic, not a very productive afternoon.

[Steve355Participant @steve355]

Coming back to this topic after several months…..

I have been using the CNC with a 1” MDF spoil board as shown, which has been ok for some operations but I need to move on.

I think I’m going to get a piece of cast aluminium tooling plate made up, 20 mm thick. it will cost a bit, but I think I need to take the plunge.

The question is, what kind of fixing holes do I need to get drilled in? A simple set of M10 Threaded holes at say 1 inch intervals?

Before I create a drawing and put in the order, I want to be sure that the pattern of holes is carefully thought through.

any wisdom appreciated!

 

Cheers

Steve

 

[John HaineParticipant @johnhaine32865]

You could overthink this.  Your proposal sounds fine, but M10 perhaps overkill, M8 or even M6 would probably be fine for a small mill.  Of course at 25mm centres!  You might also look for “CNC pallets” or “fixture plates” on eBay etc to perhaps find something ready-made.

[JasonBModerator @jasonb]

Is the machine not upto boring holes in aluminium, chamfering and then thread milling them. Would save having to get it done in which case you only need to buy in a piece of plate.

I would also consider some dowel holes and or slots so that you can drop something into them as a fixed stop which is useful to simply line up the material straight to one axis or if doing multiples you have repeatability of position much like you would with a vice stop.

[Steve355Participant @steve355]

It certainly is, at least locating the holes, which would then be guaranteed to line up with the machine. However …

 

1) I was thinking that the fixing holes for the plate would definitely be better drilled by the supplier of the plate, particularly if they are cutting it out on CNC.

2) there are some blindspots on the plate that the spindle cannot reach (probably 1/4 of the bed size at least), but nevertheless these areas of the bed would benefit from having fixing capabilities

 

 

[Steve355Participant @steve355]

Well, looks like the most cost effective way by far is to drill it myself.

Probably mark up the fixing holes using the surface plate are drill them using the pillar drill. Then use the router to  mill/drill the rest?

Any thoughts on thickness? 20mm? Or might a slimmer plate do?

[Author]

Posts