Help needed for a 3d part gcode for mach3

[JAZZCNC]

In BobCad Cam you can define stepover and cut depths for most of the 3D paths allowing you to trade off finish against time as required, the precise solution will, as you say, depend on the package chosen to do the job with.

Yes I know this has I've Been using Bobcad for 6yrs now so I know it inside out, Unfortunately it's also why I know it's rubbish at 3D.!!

however, I really don't want to over complicate things by combining 2D and 3D. I am happy to sacrifice time as I have plenty of it. at least I am not trying to do it manually 110 times as that would kill me.

Erm sounds easy and all that but in reality it's not that simple at all and with 110 of these to make then you'll soon see why combining cutting strategy's makes sense when you see the real time difference.!
Problem is that parts of your model don't suit 3D strategy's and tooling, for instance the slots have sharp corners and for an acceptable finish you'll want to use ball-nose cutter, this will put a radius in the corners. To remove this radius will then require additional operations and cutting strategy and often the cheaper Cam software's don't provide these strategy's, in this case called Rest milling.
Rest milling goes around with different size tool and removes areas that get missed by the previous tool, in your case you'd use flat bottom end mill to cut the radius away.
If you haven't got these more advanced strategy's available then your stuck with the radius or getting creative with what strategy's you have available.
Then there's the wasted time to consider, to get best finish quality with 3D paths and ball-nose tooling requires very small step-over's and has the tools get smaller in diameter the step down has to be kept lower else the tool snaps meaning multiple passes.
Getting round this tool stressing and multi passes problem then involves first using roughing strategy to remove excess material which again involves more time. So now you have 2 operations, 1 x roughing and 1 x 3D both these have to cover the whole surface area.
Then you'll still be left with the radius to deal with.!! So Even with Rest milling or other advanced strategy's like pencil milling your into 3 operations that have to cover the whole surface area. If you don't have these advanced strategy's then chances are your workaround will involve more time.!

Now if you combine 2D and 3D strategy's the operations get much simpler. The slots are simple 2D pocketing strategy's and because you can use straight tooling the corners are sharp requiring no clean up and can be cut in full depth and in one quick pass.
Same with flat areas which are simply done with area clearance or pocketing operations with same flat bottom tool and taking 50%+ Stepovers at full depth so again very quick.
This then just leaves the curves which are done with 3D strategy and roughing passes but now the area to cover is much less and confined just to the curves.
Because we have been using wider flat bottom cutter for 2D operations we use same tool for rouging. This then just leaves one tool change to ball-nose cutter which only has to machine the curves and blend into the flats.

Combining strategy's is not complicated and it's simple case of looking at the part and identifying the areas which suit 2D or 3D strategy's best then selecting the area by either defining a boundry to stay within or selecting geometry or surfaces. The Cam software you use will mostly dictate how this is done and how simple or hard to do. Better software makes this easy as clicking the surface or edges and it works the rest out for you. Others require you define a boundary calculate and apply offsets for tool being used.!!

The fact is Most parts like this require multiple operations to achieve a finished part. Combining 2D & 3d strategy's is no more complex or difficult than having multiple 2D operations like Drilling, pockets, profiling etc in one G-code file and something you'll need and want to learn quickly if doing these types of parts has the time savings are huge when doing multiple repetitive parts.

Hope this makes it clearer and don't be scared off with combining operations has it's bread and butter stuff that you'll need to learn and can save many hours or days work.

[John S]

Yes I know this has I've Been using Bobcad for 6yrs now so I know it inside out, Unfortunately it's also why I know it's rubbish at 3D.!!

What version you on Jazz ?

[JAZZCNC]

@Jazzcnc hi Dean, long post but invaluable content! For us mere mortals following this with interest but no way to open the OPs original file please, if possible, could you post one if your Solidworks renders so we have an idea what this part looks like?

Here you go Irving and yes long post but how the hell do you try to explain 2D/3D Cam in 10 words or less. . .Lol

Always with the negative waves Moriarti

Ah ah great Film and times precious in my world just like the gold in film.!!

What version you on Jazz ?

Version 24 John but only because they upgraded me Free due to there skanking sales man promising one thing and delivering another with all my protests and emails ignored.!!

[irving2008]

Here you go Irving and yes long post but how the hell do you try to explain 2D/3D Cam in 10 words or less. . .Lol

Right, now I see. Def 2D for the slots and flats and roughing out the curves, then 3D for the rest, any other approach is crazy IMHO.

Only other comments I'd add is the need for a jig to allow part to be flipped accurately and, depending on the size, consider whether several parts can be machined as one then separated in one final pass, which would decrease overall manufacturing time.

[magicniner]

Only other comments I'd add is the need for a jig to allow part to be flipped accurately.

Fixture or Jig?
A bit like the difference between cannot and may not but both important distinctions IMHO;-)

[JAZZCNC]

Fixture or Jig?
A bit like the difference between cannot and may not but both important distinctions IMHO;-)

Know what your meaning has Fixture is very different to Jig and actually often a fixture holds a Jig.!!. . . but Neither are needed actually.?

Because the slot tops are all on same plane there's a flat surface for when flipped, if the outer profile is done at same time has slots then It's a simple rectangle so when flipped new work coordinates are taken from the corner and material lower surface. No special indexing or jigs are required. . . . The Difficult bit will be work holding and even then that's not too difficult has it can be held in vice or clamped from the ends.

Thou like Irving says because of it's small size then chances are longer lengths will be machined then cut to length.? . . . . . .That's how I would do it anyway.

[magicniner]

Getting back to the OP's original request and stepping away from the Tangents this topic has spawned I've had a fiddle in BobCad Cam V25 Build 996
Before posting code I'll wait for preferred tooling size, advance per flute and spindle speed from the OP, but here's how you could get there -

1. import and reposition (translate) the model
2. Create a new layer and select it as active, then used Extract Edges From Solid to create a wireframe in the new layer, which can then be viewed satndalone by turning off the original layer (with the model in it).
3. Use Profile for the flat edge, select the line where the flat meets the vertical for geometry.
4. Use Profile to take the curved edge down to the upper vertex of the curved suface where it meets the vertical, select the line where the curved surface meets the vertical for geometry.
5 Use Pocket with outside edge lines set as dotted lines (allows the tool to pass the edge of the work) to make the operation Open Pocket for the two middle slots.

Now you're into the curved surface, you'll probably use a function requiring a Boundary and selection of the surface in the solid model layer to be selected as the geometry.

To make your boundary create another new layer, set it as active and use CAD Line drawing based on Extracted Edges to construct a Boundary for the operation, usually 1/2 the tool diameter smaller than the surface to machine.

When you Compute paths you'll get something like this -



CAM is a lot more in depth than I ever imagined before diving into CNC, I've missed out all the detail of selecting tooling options, top & bottom of work where required and multiple other options within the functions, hopefully the above shows why it's rarely the case that a request for G-Code from a solid model is met. There can be quite a lot of work for what looks like a simple job and it's rarely simply a case of feeding a model to the software and getting G-Code out,
Best Regards,
Nick