Help to make a addon for Lamello P-System Biscuits on Edge of Parts.

[ruga666]

Good Morning/Afternoon everyone,

My shop is currently planning on purchasing a Lamello P-System groove cutter w/ a P-System arbor to machine slots on the edge parts.  I don't know if anyone out there is familiar, but I just made a test cutter from the 'Slot Mill' tool option and tried to pocket the edge of a part and was unsuccessful. If anyone out there is familiar with the Lamello CNC P-System, the biscuits aren't just pocketed out, they cutter actually plunges straight into the edge of the part, moves up and down slightly then centers itself and retracts out. Here is a reference from youtube - I am trying to achieve the same machining strategy just without an aggregate on the edge of the part - https://www.youtube.com/watch?time_continue=70&v=kfoQEZV9gV4&feature=emb_logo

Also attached is my Fusion file, a screenshot of my failed set-up and a PDF of the plan/section of the Lamello plastic biscuits.  Not sure how to go about something like this hopefully someone out there is knowledgeable in doing something like this

-Sean

[ruga666]

So I haven't made much progress but figured I'd share with you all anyway.  Also I know that groove cutter was drawn at the wrong Diameter, it is actually 100.4MM and 7MM thick

But the closest I got was trying to follow a sketch line with contour, which was not friendly at all and I still don't have a way of making it go up and down without retracting and going through something.

Am I missing something or is this possibly a programming limitation and I should be using AlphaCAM instead?

If there was a way to program it to follow points instead of bodies/sketches that may work? Not sure but I am running out of ideas

I've attached a screenshot of my progress and re-attached the updated file

Any help would be appreciated, thanks

[DarthBane55]

 I think you would have to draw the entire toolpath, and use trace.  I can't think of any other method that would do this movement 😞  

[ruga666]

**** dude that wasn't the answer I wanted to hear lol.. Surely there's gotta be an easier way, what is really frustrating is if I actually cut the extrusion through both ends, the pocket toolpath does almost what I want with the exception of the Z up and down movement.

I just can't believe that no one on this forum or in the history of HSM/Fusion 360 has slotted the edge of a part for some type of biscuit or dado??!  Anyway, thanks for replying Darth hopefully someone else out there has some insight on this...?

[DarthBane55]

Ya I slotted a bunch of parts, but not like this.  I usually do a 2d contour with a couple of Z levels, but not feed in, and move up and down without getting out of the slot.  I guess you are cutting wood probably, I don't cut wood and this wouldn't work in metal I don't think.

Anyways, good luck, I hope someone has a trick for ya!

[ruga666]

I just got off the phone with the CNC specialist at re-seller of the Cutters/Arbors.  He told me that guys write custom Macros to pull this off in CAM software without having to trace lines which is what you suggested.  How would I go about finding someone who can make a add-on/button for me that would do such a thing?

[ruga666]

Assuming there is no way of doing it in Fusion 360...

[daniel_lyall]

Using the pocket toolpath will work.

Is the cutter being used? going to be able to do the cut in one go or will it need meany step-downs.

You should model the cutouts to the shape they will be cut to and the tool as well.

It is definitely doable.

[ruga666]

@daniel_lyall Yeah I figured as much. Have any other suggestions?

[DarthBane55]

---

@ruga666 wrote:

I just got off the phone with the CNC specialist at re-seller of the Cutters/Arbors.  He told me that guys write custom Macros to pull this off in CAM software without having to trace lines which is what you suggested.  How would I go about finding someone who can make a add-on/button for me that would do such a thing?

---

Maybe start a new post here, with a title like "custom macro needed" or something like that, to attract the attention of the guys who can do this kind of stuff.  I am not one of them unfortunately 😞

[daniel_lyall]

@DarthBane55 its quite easy if you use a sketch, @ruga666 can you model the cutouts to the shape they will be after being cut and post that and answer my other question.

[DarthBane55]

---

@daniel_lyall wrote:

@DarthBane55 its quite easy if you use a sketch

---

@daniel_lyall What's easy if you use a sketch?  I suggested OP to do a sketch, but it was not what he was after, he wants a custom script to output the code, that is what I can't do for him.  I would imagine that the script would not work with a sketch... or did you mean it's easy to make a script with some sort of basic sketch to start off with?

[ruga666]

@daniel_lyall Here is the file with what it will basically look like more or less after it is cut.

Yes the cutter can cut it in one shot.  As far as 'modeling' the cutter exactly how it is in real life, I don't see any options in creating a tool that would allow me to do that, at least in the slot mill options. Also, my first post shows the plan/section of the biscuit - just for reference if that helps anybody.

See attached

Thanks

[ruga666]

Oh and here's another video the Lamello CNC tech sent me of a factory in NJ doing basically exactly what I want to do if this post is not clear enough...

https://www.lamello.com/fileadmin/user_upload/Komo_P-System.mp4

[ryan]

I looked into this a while ago...developing a macro isn’t possible yet in fusion. As far as I know, the api doesn’t allow the necessary access to the cam side to directly manipulate the g-code output. Depending on your machine/aggregate capabilities you may be able to use the end mill style cutter from lamello, it’s much more fusion friendly to program vs the arbour style.

[daniel_lyall]

I am watching a video where the guy uses the Blum version, it is basically a biscuit cutter with the correct profile blade that goes into the required depth then up and down.

So in a G code, it would be, go down to the center of the cut (center of where you want the cut to be) goto the required depth into the wood (length) go up and down then back to the center back out move to the clearinces hight.

Depending on the control you should be able to get a macro done that you stick into the Gcode, or like I asked in the pm move this post to the API and Scripts page.

[ryan]

Ok here is a middle-of-the-night attempt at a workflow friendly clamex toolpath solution. I made a plug/tool component to create machinable geometry without the need for a 3d sketch. Note it does add 0.1mm to the width of the biscuit shape but that shouldn't effect the clamex performance. It will need some massaging before its machine ready but its a start.

[ryan]

*Note on the above file...the "zig-zag" in the middle of the biscuit is so narrow I may be overlooked if the tolerance value for the toolpath is set to high. It seems to work best for me at 0.00001" the setting in the file I uploaded was 0.0004" and it was being a little buggy as I was playing around with it after. As I said its a start, I'd love to see someone get this thing working reliably. It would be a nice addition for us wood guys.

[daniel_lyall]

Just write the Gcode it is a lot easier. 

%
O32123
G90 G94 G17 G69
G21
G53 G0 Z0.

(Adaptive1)
T1 M6
S7640 M3
G54
M8
G0 X100 Y100
G43 Z20 H1
G0 Z10
G0 G90 Z0
G91 Z-80
G01 Y150 F300
Z-10
Z20
Z-10
G0 Y-150 F300
G0 Z80 F300

M5
M9
G90 G53 Z0
G90 G53 X0 Y0
M30
%

[ryan]

100% the gcode is so simple. I just wish they would allow api access to position this kind of code within the model parametrically. If I had to hand code a couple hundred of these things in a project on mitered corners and all it would be a no go. +1 for api access to cam