fusion 360 cam

[geoff adamsParticipant @geoffadams14047]

I want to machine the area in blue the part is 125 mm 40 mm the boss is 25.3 dia top of boss is z zero the blue area is -.5 mm cutter 10 mm dia no matter what i try i cant get fusion to machine blue area any ideas welcome

thanks Geoff

[geoff adamsParticipant @geoffadams14047]

[Former MemberParticipant @formermember32069]

[This posting has been removed]

[SillyOldDufferModerator @sillyoldduffer]

Might be just be the picture, but is there an impossible to cut trench around the boss thingy?

Dave

[geoff adamsParticipant @geoffadams14047]

see what you guys are saying and i agree but surely there must be a way of machining this face with whatever dia cutter you like or have in your box 6 mm would do the job but using 10 mm not so many passes and does not affect anything else i could easily prog by hand

Geoff

[blowlampParticipant @blowlamp]

Is it just a facing cut?

Martin.

[Martin Rock-EvansParticipant @martinrock-evans77799]

I can't claim to be an expert, but something that has tripped me up in the past is that if the stock in F360 is set to the finished height, it won't want to machine the top surface. Maybe try setting the stock size a little higher?

[Anonymous]

It's one of those seemingly simple jobs which are a PITA. If you trying facing the system will machine the outside perimeter with no problem but will overcut the boss. Conversely if you profile between the boss and outline it won't completely machine the corners of the outline.

A simple but very inefficient solution is to profile the boss but have a number of 8mm stepovers such that the whole of the blue area is covered.

Alternatively one could create a rectangular outline more than 10mm from the outside of the blue area and profile between the rectangular outline and the boss.

Andrew

[geoff adamsParticipant @geoffadams14047]

yes it is just a facing cut but leaving the boss .5 mm high

i have machined the part using 3d adaptive clearing contour to finish the boss contour to machine outside profile and pocket to machine the c/bore but this leave part of the blue are not machined

[JasonBModerator @jasonb]

use "2D Pocket"

Select 10mm flat bottom endmill

For geometry click the face you have in blue

Set stepover at say 6mm and zero stock to leave

Press Go!

Tool will take off a series of 5mm wide cuts, blue line indicates ctr of tool axis which will automatically work out that it needs to be offset 5mm from edge of boss, you can play about with directions, stay down etc if you want

Click the top right icon on the F260 screen and select "share" then "publick link" post link here then we can play with the actual part, this is the simplified example I used which you can open in fusion

Edited By JasonB on 27/06/2020 13:34:36

[geoff adamsParticipant @geoffadams14047]

Andrew

yes simple job have come across this problem before for a simple op it seems over complicated must be a way round it your last suggestion is the way iam going to do but will use cambam an use pocket lot easy that fusion

Geoff

[geoff adamsParticipant @geoffadams14047]

thanks Jason

just tried that works great will now go an machine it new there had to be a way

ps still working on the midget engine

Thanks Geoff

[geoff adamsParticipant @geoffadams14047]

thanks everyone for your help been in the shop and cut the face Jasons post worked great

many thanks Geoff

[Anonymous]

Pocketing doesn't work in my CAM software, which is why I didn't suggest it:

It sort of does what is sensible, ie, keeps within the outer boundary and outside of the inner boundary, even if it isn't what is wanted. Presumably Fusion360 has extra knowledge of the part geometry and knows it can go outside the outer boundary?

Andrew

[blowlampParticipant @blowlamp]

Ecam does a similar job to Fusion 360 using its Contour strategy. You can either define a stock model of the desired shape or use a ready-defined block adjusted to your own dimensions.

Whilst not a 3D system, it is fairly straightforward to use and it doesn't have the learning curve of Fusion 360 either.

Unlike Fusion 360, Ecam isn't free, except at the weekend (Sat/Sun), but this might well be enough for some people regardless.

Demo video I did with Ecam's solution.

Martin.

[JasonBModerator @jasonb]

Andrew, I wonder if it is because you are selecting two boundries and not a surface? F360 won't do it if I select the outer edge and edge of the circle.

On some types of cut F360 allow you to select cutter inside, on or outside the boundaries and also add an +/- offset to any of those options

This would be another option which is actually quicker for this part, first a parallel path to remove most metal but it leaves scallops around the raised boss so a followup contour around the boss is needed to clear that up, this snip shows the cutter part way through the contour cut.

[Anonymous]

Posted by JasonB on 28/06/2020 07:27:51:

Andrew, I wonder if it is because you are selecting two boundries and not a surface? F360 won't do it if I select the outer edge and edge of the circle.

Definitely selecting a surface and the selection is called a FlatArea. But the system still highlights boundaries, so may not be really selecting a surface. Same result on a much newer demo version. Looks like it's a limitation of my CAM.

Andrew

[Alan Wood 4Participant @alanwood4]

Not sure if I have understood the problem but I would run Op 1 as a face from Stock Top to Model Top

Second op could be a 2D Contour from Model Top to Selected Contour to clear perimeter shape to bottom of overall 'keyhole' shape

Third op is 2D Adaptive from Model Top – 0.4mm (anything below model top) to Selected Contour (the top keyhole shape edge) with either zero stock to leave or some stock left for a Rest Machining clean up depending on finish.

Op 2 and Op 3 could interchange position.

But maybe I misunderstood.

[Nick HughesParticipant @nickhughes97026]

Using 2 Axis (2D) Facing in AlibreCAM gives you this:-

Edit:- "Select Flat Area" used

Edited By Nick Hughes on 28/06/2020 20:11:57

[Anonymous]

Posted by Nick Hughes on 28/06/2020 19:57:20:

Using 2 Axis (2D) Facing in AlibreCAM…………

That is interesting, you learn something every day; thanks very much.

It works fine in my old version of VisualMill:

I had in mind that using a facing operation with bosses would overcut the boss; but obviously that's not the case. I think it arose from my experiments with pockets that are open on one side. Pocketing doesn't properly finish the corners that meet the open edge. But facing overcuts the three sides that are not open. I'd better go back and do some tests.

Andrew

[Nick HughesParticipant @nickhughes97026]

To use Pocketing with an open pocket in ViualMill, you can either,

1) Select the sketch in Alibre that you used for the Extrude Cut ( you need to extend the "open side" of the sketch by more than the the cutter radius) as the Drive or Containment region

2) Create another sketch in Alibre, on the top or base of the pocket, that also extends beyond the open side by again, more than the cutter radius and select this sketch for the Drive or Containment region.

The second option would also allow you to use the Pocketing operation and get a full clean up of the edges, in the above tests.

Edited By Nick Hughes on 29/06/2020 10:16:11

[Anonymous]

I use option 2.

Andrew

[Author]

Posts