Setup

We can now move onto the actual CAM which in F360 is accessed by selecting “manufacture” from teh drop down arrow next to “design” which is the default for newly imported parts.

When you enter” manufacture” the options and icons along the top will change. Towards the left is a “setup” icon, click that and the part (s) will appear with a transparent box (or cylinder) around them which represents the stock with teh default machining allowances. You also get a dialogue box for the setup.

It depends to some extent what the part and stock are like as to whether you enter the details of the stock or the machine set up first. I this case I will do the machine setup which is basically getting the  XY&Z axis facing where you want. In the image above Z is out to the side but we want teh mill spindle vertical.

Part way down the box is “orientation” click this and you get a drop down of options, 95% of the time the first one is best “Zplane/axis and X axis” so click that

The first one to set is the Z plane which is a horizontal surface. The top is usually the best to choose, you can see that the Z arrow is now pointing upwards not sideways

In this case X is pointing along the longer length of the work which is normally how I like it but if it was not click a corner thatruns in the right direction. If the arrow points the opposite way just click flip to change direction.

If you wanted it a different way just click corner, here you can see I have clicked a corner and X has changed to what would be front to back.

With multiple parts you quite often need to tell the machine which ones you want to work on so a bit further down the box is “model”. Click “select” and then click each part you want to machine, in this case all four.

Next the details of the stock you are cutting from need to be entered, so click the next icon along the top of t hedialoge box. F360 defaults to a relative size piece of stock with 1mm machining allowance on all sides and the top.

John has a piece of 12mm plate that is 100mm x 150mm. So change the top box to “Fixed Size box” .Then work down entering the dimensions of the material. The default is to place the work in the ctr of each dimension but looking at the Carvera site it seems they make use of an “L” shaped bracket as a datum and this also has some screws to clamp the work. I have allowed 5mm to clear the screws plus 4mm for the cutter so have entered the offsets as 9mm.

The last thing to do is set the Zero datum, as mentione dit seems Carvera use the bottom left so going back to the  machine tab and coming down the list to “origin” select “stock point” and then you will see some small round nodes at the corners and ctr of the stock, click the one in the bottom left corner that is on the top of the stock.

That should be all the setup for now. Click OK.

Contour 1

On a job like this where the parts will end up being held by just small tabs it is best to do as much machining as possible while the stock is fairly solid. So the first item I would do are the four slots that pass right through th eparts.

From the 2D list of paths select “2D Contour” which unsurprizingly brings up a dialoge box titled 2D contour which opens on the first tab which is where you select the tool and set it’s speeds and feeds. As I said earlier John will have to see with some test cuts what his machine can be expected to do.  Here after clicking “Tool -select” at the top of the dropdown I have selected “flat end mill” from the right hand filter column (no longer showing) and “Milling tools (metric) from the libruarys on the left. That brings up a list of different size cutters and I selected 4mm which is what John says he has and after clicking that some feeds and speed sare listed of which I went with Aluminium slotting as most of the width of the cutter will be getting used.

Spindle speed can be altered but I think Johns should run to that, feed rate I would suggest reducing to start with maybe half to a third of that shown, some other swill change to suit, the rest can stay as is. If not using coolant, click disable.

The next tad on the dropdown can be ignored. After that the tab for Geometry can be clicked. For contours you need to select the edge of the contour, it can be top or bottom and in this case I went with bottom as they are all at the same height. The image on screen will need to be moved about so you can see what you are clicking but just one click on each bottom edge of the slot will give the four “Chains” that are the boundary of the cut.

The next tab along sets the heights. Most can stay the same but as the small machine will not be able to ramp down that quickly the feed height can be reduced from the default 5mm to say 3mm.

The other height that needs to be set is how deep to go which is the “Bottom Height” ideally the stock will have been mounted with a sacrificial layer under it to save cutting into the mill table. It does not need to be that thick, a bit of cornflake packet will do in which case enter a bottom height of -0.2mm below the selected contours which will see the cutter break through the bottom but not go too far.

The next tab is “passes” For this particular job I think that can be left as is. There are options for doing full depth finish cuts etc but I’m not sure if the machine will do those and if it did what feeds and DOC would suit.

The last tab is “Linking” bit of an odd name and it covers a few different things. Given the machine cutting by ramping down into the cut is probably the best option so click the ramp option and set the max depth as 0.5mm. Also as mentioned in teh other thread change the lead in angle from 90deg to 0deg.

That should be it so click OK at the bottom. The screen will now show the path that the tool will take. First moving down the yellow “non cutting” line, then round in an ever lowering oval to cut the first long slot. next up over and down to do the next and so on.

On 30 April 2026 at 09:51 Alan Wood 4 Said:

This means all new designs will show the blue axis vertical and you need to click on the orange plane between the green and red lines when starting the model.  The finished model will then import to CAM and for 3D printing in your intended orientation.

I think the plane you choose to start on will vary depending on the shape of the part as well as any subsequent machining or printing.

Take part like this. Both started with a “D” shaped sketch but on different planes. The smaller one would be OK for 3D printing and cutting on the CNC. However had I started the long one with the sketch on the same plane as the short one I would not have the reach to mill the profile so instead drew it on the vertical plane so the curved surface is upwards which would be ideal for scallop or parallel paths. Not ideal for printing laid flat as the layer lines will show so may have been better done vertically but that would depend on the height the printer can reach which is quite often less than the X&Y envelope. Had I tried to start sketching the long one as a rectangle on the horizontal plane it would have been a lot more work to get the elliptical curve to the top.

If you are creating a new body using surfaces from an existing model that are not parallel to the XY plane then they will also not be orientated as you might want to machine or print them. Parts created by revolving a sketch are another case where you may not want to start on the horizontal plane but the revolved part will end up orientated on the horixontal plane

Also as I said in the other thread if you are going to be machining from more than one side you are going to have to do a setup for each so may a swell learn how to reorientate now as you will end up having to do it at some point.

Bore

It was a bit of a toss up to do this first or the main contour around each part as I felt a smaller tool than the 4mm dia one would be needed to allow swarf out of the 4.2mm holes vs. getting all the 4mm cutter work done first. Th etool change and bore won out.

From the 2D Dropdown select “Bore”  And the first tab is the tool one. click “select” and choose a flat ended cutter from the metric range at 3mm dia or if imperial come with the machine select 1/8″ from the imperial cutters. As before speeds and feeds are going to be machine specific.

Onto the Geometry tab and click the inside face of each hole

Heights want to have the top height changed to say 1mm above the hole top which will allow for the stock that was left above the surface in the earlier pocket as well as a bit of clearance for good measure. And -0.2mm below the bottom so the tool cuts right through.

That is all for that one, click OK. You can see that the tool gradually moves down in a helix cutting the bore to larger than the tool diameter. Plenty of air for this one to blow the swarf out the hole.

John, Sorry I think that may be down to me. The problem of doing the CAM and images the evening before I wrote it up instead of doing it straight away.

It is the 3D section that you need to select “Pocket Clearing” from rather then the 2D “Pocket” that I said to use.

This would be the time that I would do the thread milling but as some measurements from the tool and separate practice cuts will be needed I will leave that for now.

Contour 2

With just some light finishing cuts needed to the sloping surfaces now would be a good time to cut their outer shape as that will give the finish tool room to run out at the end of the cut.

So choose Contour from the 2D dropdown. We need to use the 4mm tool for this so at the top of the “tool” tab click select. F360 remembers any tools you have already used earlier for that part so it is just a case of selecting the 4mm tool, Click select and make any changes to feeds, speeds and coolant needed.

Next onto the “geometry” tab and in much the same way as the slots click the bottom edge of each part and the whole outside will be highlighted.

Move further down to set the tabs that will hold the work in place. I changed the default rectangular to triangular, length from 4mm to 6mm and height up from 1mm to 1.5mm. F360 will automatically space tabs around the selected contouts so if you change the 32mm length that comes up to zero that will remove all the tabs. You can now go round and place them where you want by clicking along the highlighted edges . I went with two on each side of the four parts so 16 total

Next the heights tab and set the tool to cut just below the bottom of the selected contour -0.2mm

In the path dropdown click “multiple depths” and set the max to say 0.5mm which will again depend on what the machine can manage.

Lastly in the linking tab set the lead-in angle to zero rather than 90deg and make sure the lead-out is ticked to be the same. Further down click the “ramp” box and set the max depth to 0.5mm if it has not picked that up from the multiple depth setting. The Ramp height can also be reduced to 1mm rather than too much air cutting.

Click Ok and let the machine generate the path which shows the tool going round the outside of each piece while it ramps down to just leave the tabs at the bottom of the cut.

Simulation.

F360 allows a simulation of the cut which I have been using throughout to check that the paths will do what I want.

One interesting feature is that it will show any collissions and I got quite a few when I first simulated the parallel paths.

All those little red dots along the bottom are a crash and if you look closer at the image you can see some of the remaining stock (blue) has been removed as well as some of the clamps also removed (grey). This was caused by the tool holder ploughing into the material.

By right clicking the offending parallel path and selecting edit tool, then the second tab along the top “cutter” you can see why. The amount of tool sticking out below the holder is 0.2875″ or 7.3mm but we are cutting almost to the full depth of the 12mm stock. Easy enough to change but it is something that needs to be checked for each tool you use and make sure when you mount the tool it is sticking out at least as far. The same goes for cutters with a larger dia shank, you need to get them entered as they are. For example a 1/16″ cutter is quite likely to have an 1/8″ or even 1/4″ shank and the 1/16″ part will not be very long.

related to that F360 will only throw up crashes into the stock you have entered (unless you model your vice, hold downs etc) So if you have screw heads or clamp plates bearing ontop of the stock you also need to take their height into account.