CNC Profiling

[JukeSnowboarding]

I am stilling learning the ins and outs of using a CNC machine. So far cutting the core and drilling the inserts seems simple enough, but I dont even know where to begin with profiling the core.

Not sure how to go about creating the toolpaths or even design the profile.

Any advice or tips would be greatly appreciated.

Thanks,

Tim

[JukeSnowboarding]

Believe I found my answers buried in the forums. Woo

[MontuckyMadman]

Sweet drop some links here

[switzch]

Hey Guys - Can anyone shed some insight on what you are doing for toolpaths specific for profiling? I have founds some solutions using vectric software but im not happy with the solution and would like to see if there are other easier solutions on there.

[switzch]

I have been using sketchup to make the profile and then importing the dxf into aspire to generate my toolpaths. Have had some success but wondering what others are using from a software standpoint to generate tool paths?

Also curious what people are using for feed/speeds? I am using a 1.5" bottom cleaning bit for profiling taking 0.05" at a time at 80-100 inches per min. Takes about 35min per core.. probably could speed things up but not sure what to change to optimize things.

Super new to the CNC world and learning over the last few months. My setup is mainly profiling bamboo with a CNC Mogul and a 2hp craftman router.

[MontuckyMadman]

Have you tested just upping the feed rate? Depends on the core size prolly get that down to 27 min per. The mogul might have a limit and you might be at it.

Have you considered useing a horizontal roughing pass to start, removing more material, and switch to a parralel fiishing for the last few steps?
To me that sounds like a really big bit, more like what you would use to surface the top as opposed to cut some fine cores.

[twizzstyle]

I use a 1.5" bit and do a roughing pass just as montucky described, followed by a lengthwise finishing pass. All at 75ipm.

[switzch]

I have a roughing pass but it still runs parallel with the length of the ski. I will try changing it up to a horizontal pass.

I use a 1.5" bit and do a roughing pass just as montucky described, followed by a lengthwise finishing pass. All at 75ipm.

Questions;
- How much do you take off on the roughing tool path per pass?
- How much to you leave for the finishing pass?

[amidnightproject]

i do a horizontal roughing pass and a vertical finishing path.

I was using a 1.5" flute bit. Just switched to a 4 flute 0.5" endmill. Much faster and better results. Down to 22 minutes for a 124-108-113m 186cm

Roughing pass at 180ipm. Finish pass at 100ipm.

I take off 5mm on the roughing pass. then no more then 3mm on the final pass.

[Cornice]

I use cambam witch is not my favorite so far. I had been exporting the side profile from Snowcad into my cam software. I then extrude it and re-align. Now i draw the profile in cad.

The last core i profiled was
cut at 2400 feed rate
double flute 19mm bit
7.5mm step over
all depth in one pass

This one worked on one core and the other blew the sidewall off. I think my step over was way too much.

[ben_mtl]

your stepover is fine.
I would guess the problem is you take too much material, too fast. Try doing it in 2 passes. I would keep the feedrate as is, you could even increase it if you make shallower passes since the stress on the machine will be reduced.
I would not try to decrease the speed and keep a "1 pass" machining, you'd risk burning your core and your cutting bits. I tend to always put the priority on feedrate rater than DOC.

BTW I too use Cambam, while it's not perfect and not necessarily very user friendly I find it pretty nice and have yet to find something I'm not able to do with it.
Lots of tutorials on the internet, there's even a script to create DragKnife toolpath from any geometry. I've developped a few scripts that automates the importing of my CAD file -» distribute / moves the geometry over multiple layers -» create the basic machining operations... saves a lot of time and reduces potential mistakes !
I dont' use snowCAD though.. I design all my skis in 3D with Catia since that's the software I use for work, then I made a scipt so Catia creates all the toolpath I will need for machining. I just design the outline of the ski, the script then creates all the geometry to cut the bases (taking into account the length of edge I will need so I have edge tines at both ends of an edge length...), the cores, the chanels for PU sidewalls, tipspacers if needed, it adds inserts for bindings at the right position (I choose the bindings models + mounting offset from a menu) and a few other things.
Then Catia exports a DXF file with the 2D geometry and an STL file for the 3D profile operation in CamBam.

[skimann20]

what type of bit is this!?

0:13-0:14. looks narly!

[twizzstyle]

That's a roughing endmill, used to take off lots of material but leave a not-so-great finish. Good for metal, not sure it's really needed for wood.

https://www.google.com/search?site=&tbm ... jlgYzGsaLA

[skimann20]

it probably leaves a nice surface for them to bond their UHMW Sidewall too. I've been looking for a better bit than my two flute straight bit to cut the core shape out with. The bit seems to gain to much heat when I do it. Last core i tried a spiral upward bit and it did much better but I'm still looking to see what others are using.

[twizzstyle]

For cutting out shapes I use a 1/4" down-cut two-flute. The down-cut keeps the work pieces from lifting, that's the main reason I use it. Has worked great for me! For profiling I use a big 1.5" straight flute router bit.