View Full Version : Having a go with F360....

11-08-2016, 08:09 PM
Ok, so I'm average on Vectric Aspire and SheetCam but want to learn basics in F360 - i like the assembly stuff and 360 aspect of design that the other apps lack.

Have watch a few videos but find the best way to learn is to pick something representative of a project either past or future and try designing it.

Here we go, not to any scale and only the first steps of the part.


I drew the stock, added two circles and then the slot on one.

Doing the cam and a simulation it wants to cut round the whole part - presumably because it is following the path through the slot.

Say i wanted to mill the holes out then do the outside then add the slot, what process should i be following?

Would the slot be a separate setup or separate file/code etc?

Apologies for basic questions but searching for this would probably take a long time ;)

12-08-2016, 09:26 AM
Several hours of the 'tube later ;) i have found an answer - draw another circle on the top plane and machine that instead of the actual hole - simples.

12-08-2016, 03:08 PM
Ok, so its been a quiet day in the day-job today but couldn't sneak home to work on the project as it was my watch as they say :fatigue:

Been playing with Fusion360 :joyous: Sort of come up with a plan for the top plate of my dual-spindle adaptor for the mill. My thoughts are in the machining process...

Spot the three holes in the middle,
Drill them through,
Counter-bore them,
Rough pocket out the two big holes,
Finish pass on them,

Questions so far,

should i rough the holes then finish with a mill tool or should I go for the boring head and bore-gauges/caliper ??
I was thinking to then flip over in the vise, mill the slot on the rear face, then flip back, bolt to table on scrap pads through the big holes and do the outer contour followed by the two small slots and a chamfer pass?
How to chamfer the rear face once contoured?

So far its been a blast, love the 360deg view :joyous:


12-08-2016, 06:28 PM
Sorry I can`t be of more help mate, I`m still just getting to grips with F360 as well ! You seem to be making good progress though for the short time you`ve been using it:cheerful:

12-08-2016, 09:45 PM
Depends if you are making out of an oversized block or plate that is already at the correct thickness.

If using plate I would use a another piece of plate underneath as a fixture, clamp at both ends then....

Mill slot and drill holes(making sure to drill into plate below,
Interpolate two large bores with a slot drill and chamfer
Use a T shaped clamp in both bores to hold while milling the profile.

Then put a couple of pins or drills in the holes and use them to align the part when you flip it over.
Clamp with T clamps again.

Counterbore and mill the two slots that break into bores.

13-08-2016, 08:20 AM
Thanks, not thought about a fixture below with the alignment holes :)

I was going to use precision tooling plate, used it before and accuracy has been good on thickness.

What about bore finish - mill outright or mill rough and boring head? Its a consideration because of the massively different clamping methods needed for a using a boring head.

I don't think ultimate precision is needed, i was allowing +0.25mm clearance on bores, maybe more?

13-08-2016, 09:45 AM
I have been using the tooling plate a lot recently too and have also found the thickness and flatness really good.
I just use another piece of tooling plate as the fixture.
Using a milling cutter would be fine to finish the bore. If you were making a batch I would say use separate tools for roughing and finishing though.

13-08-2016, 11:55 AM
Thanks, when i get the mill up and running this will be one of the first projects - a real "pucker-up, suck it and see" moment i think. ;)

Will use a mill tool, probably change though as the pocket will be ripped with a two-flute and finish passes are better with three or four flute tools.

19-08-2016, 09:39 PM
Top and bottom plates drawn, just the spacer block left.

The smaller hole in the bottom will take a 20mm spigot that will lock into an R8 collet in the spindle.


Metal arrived today and the mill is almost ready to go.

24-08-2016, 07:50 PM
Ok, first job :)

Something i used to make manually in small batches, would use a 5C collet block horizontally in vise, cut one side, rotate 90deg cut next and so-on. The diameter of the tool created a radius at the root of the square part.


Gonna have a go with CAM, modified the vise jaws so i can clamp a blank vertically and work round tip using a ball-nosed cutter.

Blanks are 1/2"dia and tip is 5.5mm sq. It also 605m36 steel so slightly harder than plain mild.

I have it drawn up in F360 and worked out the feeds/speeds in HSMAdvisor which gave me 420rpm, 84mm/min on a 12mm HSS tool. DOC is 11mm - 6mm radius and 5mm straight.

F360 wants to take the whole cut in one pass - would you feel happy with that, seems heavy. Although i selected 2d Adaptive, i think its too simple to work any magic on and it seems to have created a standard path.

29-08-2016, 10:58 AM
Ok, back to this task, nearly ready to get cutting now :)


My thoughts are to fix the waste strips down to table,
set plate square to axes,
clamp plate on top,
mill the slot
drill the three holes tapping size through
drill the part holes to clearance size
tap the holes in the scrap and bolt part down
remove clamps
mill the two large holes
mill the outer profile
flip over and bolt down
mill slots
clamp part again
remove bolts and counterbore three holes.

I think that maintains accuracy between the slot/holes and the two big holes??

I could maybe add two extra holes between the three bolts for 6mm dowels if needed?

The bottom plate will be easier as i only have to drill the three bolt holes and maybe dowel holes and then clamp down using the same offsets for the part.

29-08-2016, 01:18 PM
I think you're over-thinking it ;-)
Square your stock and drill & tap the clamp holes manually.
Stick it in a vice on parallels with thin sheet sacrificial spacers on top and machine all the internal features, including slot.
Hang it out of the vice to profile and slot one end outer curve, flip and repeat.

29-08-2016, 01:48 PM
It won't fit in my vise though :)

29-08-2016, 03:32 PM
Ok, work holding issues aside, say i have machined the inside features etc and want to create the outer contour...


F360 knows the exact size of the raw stock but I'm buggered if i can figure out how to create a path to machine the junk away??

Do you need to draw a box/path around the stock - if so whats the point of putting the stock size in?

You cant select the stock in a process so i cant see its point?

31-08-2016, 08:42 PM
F360 is doing my head in ;)

I have my front face set up with my chosen work coordinates system (WCS) as front left corner, Z is of course up/down.

Now, i presumed that if i wanted to machine a feature on the bottom or underside face of that part i could rotate it round, do a new setup and set my WCS as top left corner with Z again now being upwards???

I have spent an hour messing and given up for now - it will not let me position the WCS how i want it and persists in putting either the x or y axis in the wrong direction, i post processed a trial and it does not work as it is off the table in Mach3.

Any ideas how to machine stuff on the underside of a part???

01-09-2016, 08:54 AM
It seems it is correct and the error is my brain and Mach3's tool path display.

So far all my work has been done in Q1 which is pretty normal and has home at bottom left corner, the work on the reverse side is in Q4 with home at top left - this seems to make the tool path display hang it off the bottom of the screen which made me think it was wrong.

I sketched out the four quadrants and pencilled in the first few G-code lines and they do indeed fall where they should :)

I will have a play on the machine tonight and do a dummy run.

03-09-2016, 07:37 PM
To fix the display issue, you have to turn off "Table Display" in Mach3 :)

Next -

I have code for a part that needs to be run as batches - same code with a break to reload the stock.

How do you stop the pointless tool-change but still maintain the tool length offset??

Code starts like this...
(T1 D=12. CR=6. - ZMIN=-10. - BALL END MILL)
N10 G90 G94 G91.1 G40 G49 G17
N15 G21
N20 G28 G91 Z0.
N25 G90

N30 M5
N35 M9
N40 T1 M6
N45 S650 M3
N50 G55
N55 M7
N65 G0 X-2.546 Y13.069
N70 G43 Z10. H1
N75 Z2.
N80 G1 Z1. F180.
N85 Z-8.8 F135.
N90 X-2.54 Y13.063 Z-8.934