Going over to the dark (CNC) side!

[Jasonb]

Achim, I got the vectric thrown in for free so that was really my only reason for using it and it seems quite simple to use. Although I draw in Alibre I had already looked at teh F360 CAM and will give that a go now that the machine seems to be behaving itself. I have already imported some STL files from alibre and done some simulated cuts to get curved surfaces (in Z) which you can do with a DXG file in Vectric Cut2D.

[kvom]

FYI.  Cambam can do 3D surfaces and supports molds, where the positive surface is inverted in Z.  One of the most active members on the CB forum has a business making molds for fishing lures.

One thing that CB lacks at present, that other 3D CAM software may have, is "rest" machining.  The simplest type of 3D machining is a roughing pass for which one can use regular endmills, and the finish pass where a bullnose type cutter is needed.  What one would like ideally in some cases is two or more roughing passes where extra passes can use smaller tools to get close to the desired surface;  in other words, roughing the rest.  If that feature isn't present, then the machine spends much of the time cutting air on the second pass.

One needs to be careful with STL files found on the internet, as they may have problems that CAM programs can't handle.  There are several programs available for repairing the meshes on STLs.  Meshlab is one I've seen recommended.

[jadge]

The USB stick for V2.x is $24.95; I've ordered one. Unexpectly the order went through with 'free' postage.

I received the USB stick today. It was indeed free postage. But I got stung for £20.57p by ParcelForce for import duty and "handling" charge. Not so much force as darn right extortion. 

Andrew

[Jasonb]

It is all well and good cutting random shapes into bits of scrap to get the feel of things but nothing beats making more productive swarf. To this end I have been drawing up the next stationary steam engine for a while and was possibly going to get a couple of the parts laser cut but now that I have the CNC what better way to learn and be productive at the same time. The base "casting" of the engine will be a sandwich of 3 layers so I started with the bottom one, the upper is similar but has some different holes and bosses.


A Step file of the required part was exported out of Alibre and into a F360's CAM program where I generated the G-code for the holes and the actual shape as separate sets of code to make it easier for me rather than have to incorporate tool changes. I air ran the code first of all and then again into some PVC which showed up a slight error in heights which was corrected before cutting metal.

I started by clamping the stock onto some MDF and first ran code for eight 3mm holes, then after changing bits ran another code to enlarge four holes to 6mm. After that these holes were used to screw the 2.5mm thick plate to the MDF so that the clamps could be removed. After changing to a 6mm 3-flute HSS FC-3 cutter the button was pressed. I'm more than happy with what came out for my first proper part using CAM and the first time cutting steel and this plate is a bit gummy.

A couple of areas did not quite cut all the way through which was probably due to the scrap MDF that had been sitting around for a while but that just tore away. You can also see that I left some 1mm thick tabs to stop the larger pieces of waste moving about.



After a quick clean up

[Admiral_dk]

Looking good Jason 

I can't say that I'm surprised that you had a few places that didn't go all the way through ....

When I use the small CNC-Router at work, I use a template cut in high quality plywood that holds an Euro-Card PCB (160x100mm.) and even though the router itself has cut that pocket, I still get small variations.
This means that if I need to cut the PCB to a "strange" shape when all the rest of the milling is done, I let the cut go aprox. 0.5mm into the wood in the pocket (except the tabs) in order to ensure a clean cut-out.

[kvom]

Does the single STP file encompass all sides of the part?  If so, how do you select the view and edges that encompass the machining?

In SolidWorks, I select a view of the part and export a DXF of that view.  For 3D surfaces, I export STL.

[Jasonb]

Yes, it comes out as a complete 3D part in F360 so I can pick any feature as the geometry to cut. You can also select what way the part will be orientated on the machine if you did not draw it with the axis in the best position for machining. You can also enter the size of the stock so it knows what you are starting with.

This is the imported part showing the path of the tool and the second picture shows the end of the cutting simulation with the stock shown

This series of videos are what I used to see how to do it with F360

<a href="https://www.youtube.com/watch?v=6FzbZNhey2w" target="_blank">http://www.youtube.com/watch?v=6FzbZNhey2w</a>

[Jasonb]

I had a bit of time this afternoon so thought I would do the top plate, I did not air cut this time but did practice on some PVC before cutting metal.

First was to drill 15No 2.5mm holes with a split point stub drill which meant I could get away without spot drilling first



Then a change to a 6mm stub drill to open up six of the holes



Using these holes the plate was screwed down to the MDF below and clamps removed. Using a 6mm dia 3-flute cutter but carbide this time the profile was cut, not a bad finish on the bottom of the first pass.



All complete, the 6mm piloted holes that open out to the edge were enlarged to 8mm as part of the contour cut and I left tabs again to stop the waste flying about.



After a clean up with the bottom plate that I cut at the weekend.



I've stitched two videos together here, the beginning shows the first pass with the cutter at full width but 1mm away from the finished edge, second half shows the final full depth finishing cut, you can see the tool rise and fall where the tabs are located. The upload to Youtube seems to have added some high pitch noise which was not there at the time.



I could quite get to like this CNC lark, next part has been through the CAM and will let me try some adaptive clearing cuts!

[kvom]

You could have added additional screw holes for the 3 extra pieces, and then avoided using and cleaning up the tabs.

Another hack that can save time is to use center cutting endmills for drilling.  In this case a 2.5mm tool could be used to spiral drill the 6mm holes.  That saves a tool change, but here you needed the 6mm tool for the next op.

[Jasonb]

Funny enough I was thinking the same about the extra holes as even with a ctr cutting bit and a slow plunge the drop down after the tab was the one item where the cutter did not seem happy.

Not tried spiral cutting a hole yet but hope to give it a go soon.

[kvom]

Spiral cutting is especially useful when you don't have a drill of the size you need.  Plunge milling makes a lot of sense for  roughing deep pockets; the Z axis of mills is almost always stouter than the X or Y, and there are no lateral forces to bend the tool.  In place where you might do chain drilling, you can plunge mill at less than a 100% stepover.

I usually make my tab length 3x the height.

[Jasonb]

The adventure continues with this part which will be the bottom mounting flange of the cylinder.



First operation was to run the code which put the four 3mm holes into an oversize piece of 1/4" flat steel bar. I then put an offcut of aluminium into the vice and ran the code again but this time with a 2.5mm drill, the holes were then hand tapped and the two screwed together without removing the aluminium tooling plate from the vice.

With a 6mm dia 3-flute carbide cutter I first ran an adaptive clearing cut around the outside followed but a final contouring cut to finished size. I started off quite tame at 3000rpm and 150mm/min feed but found that could be upped as the flat bar cut a lot better than the steel plate I was cutting the other day.

The next part of the code had the adaptive clearing to form the 4 raised bosses, this again had been programmed as above but found I could go faster and ended up at 3900rpm and 225mm/min feed.

Again Youtube has added some high frequency noise but you can see the first cut around the outside where the DOC varies as I only rough centered the work followed by 3 clips of the top clearing at various stages.

<a href="https://www.youtube.com/watch?v=dd4sHBimQ-g" target="_blank">http://www.youtube.com/watch?v=dd4sHBimQ-g</a>

Final job was to skim the bottom off, final size will be done after silver soldering the assembly together.



Intention is to have a 20mm block between the bosses so a quick test with an ARC 10-20-40 block to see what the fit is like



Can't get much better than this

[kvom]

Why is the return move on each clearing cut so slow?

[Jasonb]

Why is the return move on each clearing cut so slow?

Because I still have a lot to learn

I have now found the box where the "non engagement feed rate" can be set, looks like it defaults to the cutting feed rate so I have now increased that and will know it needs to be done the next time I use the Adaptive.

Out of interest do you set the speed of these return movements the same as the rest of your rapids or less?

J

[Jasonb]

Over on ME Forum I have also been advised to set the adaptive to cut in both directions which makes it quicker still, I had just been using climb cutting.