F360 stock from solid

[Roderick JenkinsParticipant @roderickjenkins93242]

I felt it was time I exercised my little CNC milling machine, originally a Sherline based Denford, now converted to Mach 3.  This little machine can only take light cuts so takes an age to produce anything. It occurred to me that if I could take 10 minutes to rough out the shape I wanted to make on the bandsaw, this would save a great deal of swarf or air cutting time since, by default, F360 assumes a rectangle around the part .  It took me a couple of days of scouring Youtube videos to work out how to use this rough shape as stock in F360 but eventually the penny dropped.  The trick, it seems, is to design the shape of the stock and save it as a mesh.  This mesh is then inserted as a body into the project at the design stage.  This body can then be selected as a stock from body option in the manufacture stage.  At least, that’s how I got it to work.  In my case I made the stock 4mm larger all round the profile.

 

 

 

I printed the stock profile and stuck it to a piece of ally and had at it with the bandsaw.  So long as the cut was within the 4mm excess then the quality of the cutting shouldn’t matter.

I used the blue masking tape and superglue method to stick the blank to the fixture plate on the mill table and cut the profile with a 6mm 2 flute polished HSS endmill.

 

My cunning plan was to take advantage of the fact that the ally plate I used as stock was 30 thou thicker than I needed so I would be able to turn it over and skim it to the correct thickness on the manual mill.

Not so cunning then!  I got my depth wrong somewhere and to add insult to injury the superglue bond gave way just as the final finishing cut to the profile started.

So, not a complete disaster.  I’ve learnt something about F360 and also that the CNC mill is more capable than I have given it credit for, although I think I was a little too aggressive with the feed rates which may be why the part pinged off with a full height cut.  Although the result is 0.2mm oversize because it didn’t get the finishing cut, the final product is entirely usable.  Anybody know what it is?

Cheers,

Rod

 

 

[David SeniorParticipant @davidsenior29320]

It might be worth checking whether the depth error was a number error by you, or whether the cutter was pulling out of the holder. It’s certainly a problem that I have had.

Dave

[renardiere7Participant @renardiere7]

The closest I come to CNC is cutting out intricate profiles on my pantograph but it occurs to me that the same principle applies here to reduce the cutting load as you have done.

[JasonBModerator @jasonb]

Rod, another simple way to do it is to first create a 3d ADAPTIVE around the part with say 3mm radial stock to leave  as the first operation which will effectively produce your sawn part.

You can then do the actual contours or adaptive cuts and simply not run the first Dummy adaptive. The CAM thinks it has already removed what you have sawn off so the other paths will not try to cut air.

Something like this

You can also use a “model” as the stock which would just be a modified version of the part with a 3mm border around it. but that is more work

[JasonBModerator @jasonb]

This one was done as above just a dummy cut to leave 3mm around the shape. You can see the cutter starts to cut where the saw cut is furthest from the final contour and with each pass takes a bit more off.

I also use the same method on flywheels where I may drill a big hole between the spokes before using the CNC. Or again with flywheels as I do the turning first on the lathe if the hub sticks out beyond the edge of the rim I will just use a solid cylinder for the setup and then run a dummy contour or adaptive across it to bring the heights to the right level for the actual turned part, leaving the hub spigot standing proud.

 

[FatgadgiParticipant @fatgadgi]

I’ve always taken the idiot’s approach and used 2D Contour, leaving radial stock before the finishing cuts.  Effectively cutting a slot around the profile with clearance. I don’t always cut in one go, sometimes half the depth before adjusting the clearance, and using a 2 flute cutter.

I did once try using a Model as the stock – seem to remember it wasn’t worth the hassle, so didn’t try it again.

Cheers Will

[Roderick JenkinsParticipant @roderickjenkins93242]

So many ways to skin a 🐈   The obvious way to cut a profile is just to plough around the outline but my machine doesn’t really have the rigidity for that together with the swarf clearance issue makes me disinclined to use that method. However,  much food  for thought.  And Dave,  I think you may be right about the cutter pulling out.

Thanks guys,

Rod

[Neil LickfoldParticipant @neillickfold44316]

You really do need a flat plate with no added holes to glue the parts to. The total bond strength is far greater that way. It is handy to have a pad and a screw thread behind it for removing a thicker section part. With super glue hot water will usually break the bond.

As the temp of the bond increases, from room temp, the strength declines with super glues. So it pays to ensure that the part is not getting over 40c or so for best results.

Glad you found the cause of the problem, with the cutter pulling through.

[John HaineParticipant @johnhaine32865]

I stick the part directly to an ali backing plate if I can and boil to separate. And / or use holding tabs.

[JasonBModerator @jasonb]

I put tape on both parts. When I come to take the job off it is the tape joint that breaks so any glue is left on the tape and no need to clean it off the work or machine. Do you have to take the whole backing plate off the machine to boil?

Double layer of tape also gives you room to have the cutter go just below the bottom of the part and not as far as the plate. Screws added after the engraving but before cutting the oval.

 

[John HinkleyParticipant @johnhinkley26699]

I’ve  never tried the blue tape/superglue/blue tape sandwich method myself but I have used 3M VHB double-sided tape to great effect when used on my cnc router table for aluminium.  It sticks like nobody’s business and unless used quite sparingly, is annoyingly difficult to shift.  It would take a seriously over-enthusiastic cut to dislodge it.  A more likely outcome would be a broken cutter!

I use 20mm wide stuff for various jobs around the shop most satisfactorily. It is about 1mm thick once applied, so consequently will also allow the cutter to clear the substrate base whilst taking full depth cuts.  I also recommend small tabs. It isn’t cheap but will do the job without the need for heat, solvent or boiling water.

(The seller that I have pointed to in the link above is not the one I have bought from, it is just an indication of what it looks like – the red backing peels away after applying to the stock to reveal the sticky gel with which the stock is  attached to the machine.)

John

 

[NealebParticipant @nealeb]

Never thought of the “dummy first cut” technique – sounds really useful, and particularly if dealing with machining a casting to avoid “cutting” bits that don’t actually exist. Another one for the CAM toolbox – thanks!

 

[JasonB]

On JasonB Said:

I put tape on both parts. When I come to take the job off it is the tape joint that breaks so any glue is left on the tape and no need to clean it off the work or machine. Do you have to take the whole backing plate off the machine to boil?

Double layer of tape also gives you room to have the cutter go just below the bottom of the part and not as far as the plate. Screws added after the engraving but before cutting the oval.

 

 

It’s preferred, otherwise you need a rather large cauldron…  The steppers etc are also a b****r to dry out.

I find that the glue layer usually comes off as a separate film, or if not is easily scraped off.

[Roderick JenkinsParticipant @roderickjenkins93242]

Against my (clearly poor) better judgement I’ve tried a profile cut.  3mm 2 flute bit at 8000 rpm works fine at 1mm depth per pass and 200mm per min.  Machining time 16 minutes which doesn’t seem too bad.

On this pulley it would be nice to do a chamfer on the spokes but F360 personal won’t let me change tools.  Does anybody have a strategy for copying the part to maintain alignment for a second operation?

cheers,

Rod

[JasonBModerator @jasonb]

Rod. Do all the CAM on one single part roughing, finish contours any drilling, chamfers etc. When you have them all listed down the side click and highlight the ones that use the same tool and then do the post processing. Repeat for each path/tool type. If you just try and do the post processing for the lot you will get the warning come up about personal use.

 

All you need to is run the first one on the CNC with the required cutter. Then change cutters & set height then run that path and so on. Just keep your X& Y datum the same. I do it all the time like that. You can see here I have created a lot of NC Programs (post process) not only for machining from two sides but also drilling the mounting plate used to hold the part in place. Just copy them all to a USB stick and work through them.

 

If when you were designing the part you rounded off the spoke corners with a fillet then you could cut the filler with a seties of cuts using a ball nose tool to give round or oval spokes.

[Roderick JenkinsParticipant @roderickjenkins93242]

Thanks Jason.  That works.

Rod

[Author]

Posts