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]

Thanks @daniel_lyall and @ryan -

Couple of things, first of all thanks for putting time and effort into the issue it is greatly appreciated and part of the reason why I am a Fusion 360 advocate.  As far as woodworking and getting this to become an easy properly working feature, I think yes this is a big deal and will blow open doors for all the woodworkers out there using Fusion 360.

I have contacted NexGenCAM who wrote the post for my aggregate just to see what they had to say about it, and there response was Yes they can make it work, but it would be something that would have to be worked around in the post processor which obviously doesn't benefit the Fusion 360 woodworking community.

Like you said @ryan in response to @daniel_lyall  - Sure, I could copy and paste some g-code around and get this thing to work but I'm machining possibly 50+ of these per sheet on all sorts of different shaped and sized parts on many different sheets. So in this particular case that will not work.

@daniel_lyallif you could move this post to API & Scripts so that we could get some insight from someone out there that would be very helpful.  Appreciate everyone who's responded and put some thought into the subject

Godspeed

[ruga666]

Thanks @daniel_lyall and @ryan -

Couple of things, first of all thanks for putting time and effort into the issue it is greatly appreciated and part of the reason why I am a Fusion 360 advocate.  As far as woodworking and getting this to become an easy properly working feature, I think yes this is a big deal and will blow open doors for all the woodworkers out there using Fusion 360.

I have contacted NexGenCAM who wrote the post for my aggregate just to see what they had to say about it, and there response was Yes they can make it work, but it would be something that would have to be worked around in the post processor which obviously doesn't benefit the Fusion 360 woodworking community.

Like you said @ryan in response to @daniel_lyall  - Sure, I could copy and paste some g-code around and get this thing to work but I'm machining possibly 50+ of these per sheet on all sorts of different shaped and sized parts on many different sheets. So in this particular case that will not work.

@daniel_lyallif you could move this post to API & Scripts so that we could get some insight from someone out there that would be very helpful.  Appreciate everyone who's responded and put some thought into the subject

Godspeed

[ruga666]

sorry didn't mean to post that 2x

[ruga666]

I've noticed that this post has attracted an awful lot of traffic, so I'd like to give everyone an update-

I've been in contact with Bruno and Ben from NexGenCAM.  Bruno has created a Lamello P-System library part in SolidWorks that you insert onto a center point on a sketch and allows you pick what side gets the fastening hole, if you'd like to rotate it on an angle etc. He sent me a video of him inserting and programming one to show me and it appears to be relatively easy. See attached screen shots

Unfortunately, we're using Fusion 360 and we don't have library part features.  So they've contacted Autodesk directly and are going write some sort of add-in for Fusion 360 to get it to work the same way.  So anyone who has been waiting for this, it's actually in the works!  We also discussed how nice it would be if Fusion themselves added some sort of feature that allows you to click and drop these things around the edge of parts similar to adding Tabs - Fat chance!!

[ryan]

Thanks for the update! Beyond just lamello, the ability to drop in and position user-programmed (geometry and Gcode), like tabs, as you said, would be a huge step forward in fusions production/manufacturing functionality; especially for millwork and furniture. Hopefully the developers at AD will take notice and fast track this if its not already on their roadmap. Keep us posted on the add-in, this got very interesting!

[ruga666]

I agree 100% Ryan, if they did implement some sort of way user modeled/programmed geometry like we're talking about, this program would literally be taking things to another level that no other manufacturing software has done before.  Hopefully the right people are reading this post and someones getting the ball rolling on some of these ideas!

[pludikar]

Hi,

I just thought I'd try and throw in my 2 cents/pennies worth, and offer a potential work around to do this before someone creates an Add-In.  I'd also suggest that the slightly more Fusionistic way to do this is to:

1. Create the shape of the Lamello cutout and keep it in a separate file.  Include a joint origin at the centre
2. Import the Lamello cutter shape into the furniture/Cabinet model
3. Place the lamello shape onto the part using joints and their offsets
4. Either use pattern to place more shapes on the part, or Copy and paste and joint-place subsequent copies of the lamello shapes to where you need them.
5.  Combine/cut the lamello shapes into the parts (if you have two parts that need joining and are already modelled in the right place, then you can cut the lamello shape into the other parts as the next step
6. Go to the Manufacturing workspace
7. Once you have a setup ready, add a contour  operation
8. Assuming you have already created a custom form mill of 100.4mm radius and 7mm high, select the contour geometries 
9. Under leads and transitions, enable Lead-In and Lead-Out, and make Lead-Out same as Lead-In.  Make Horizontal Lead-In Radius = 0; Lead-In Sweep Angle = 90 and Linear Lead-In Distance = 1 in (You will probably need to fiddle with these to optimise) 
10. Set Finish feed rate to something easily recognisable (eg 30 in/min) and different to other feed rates (eg 60 in/min).  You will end up with a path like this:  
11. Post the toolpath.  Edit the resulting GCode file - Add a Macro routine to do the up/down jiggle (How you do this will depend on the machine you have, and assumes that you are only cutting in the X/Y plane). Do a search for F30. (in this example case) and replace with F30. Mxxx (where xxx is either a Macro Line number or a Macro file, also dependant on your Machine).  

(2D CONTOUR1)
M5
T7 M6
S5000 M3
G59
G0 X12.3512 Y-4.7715
G43 Z0.6 H7
G1 Z0.25 F60.
Z-0.5118
X12.8606 Y-3.9109
X12. Y-3.4016 F30. Mxxx
X11.1394 Y-3.9109
X11.6488 Y-4.7715 F60.
Z0.25
X3.3512
Z-0.5118
X3.8606 Y-3.9109
X3. Y-3.4016 F30. Mxxx
X2.1394 Y-3.9109
X2.6488 Y-4.7715 F60.
Z0.25
X21.3512
Z-0.5118
X21.8606 Y-3.9109
X21. Y-3.4016 F30. Mxxx
X20.1394 Y-3.9109
X20.6488 Y-4.7715 F60.
Z0.6

M30​

In theory that ought to be it, but I can't be 100% certain that this approach will be robust enough to cope with all scenarios - but at least I think it's an approach worth exploring.  I'm hoping the F360 will have a more meaningful API to CAM in the near future, in which case creating a script to do all of the above wouldn't be too onerous - at the moment creating a script to do everything up to the CAM part is relatively easy - I've done a dogbone Add-In that uses a similar approach.  I also suspect that the up/down jiggle GCode macro call could be added in the Post processor for your particular CNC machine.

Any way I've attached the cutter model and the test part, in case this is of interest.

Peter

[ryan]

I like the idea of a search-replace with reserved feed rate "markers," I think this is probably not far off how the OP was going to have this accomplished in a custom post-processor.  For basic z axis tool orientation this would work very nicely. Even in x/y you could create two more gcode blocks and use three different marker feeds. However, it will get significantly more complicated when positioning on miters and off axis tool orientations (a very common application of this connector). It's mathematically possible with some conditional trig functions but I think this would require more associativity with the model than editing the gcode output. Great work around for x/y/z though! 

[pludikar]

@ryan 

Can I assume that, because you want to cut the slots in mitres and other angles, that you have a 5 dof (degree of freedom) CNC?  I'm not an expert in 5d gcode, so others will probably confirm or shoot down what I'm about to say: 

The basic premise of gcode is that the plane of operation has to be defined (whether by default or otherwise), and x/y/z is relative to the fixed cutter spindle axis.  If you are operating in the typical x/y plane, depending on your machine setup, the gcode instructions are going to be either absolute (specific x or y coordinates in the desired plane) or relative (incremental coordinates, with gcode G91 X1 resulting in a 1 inch movement in the x absolute plane).  Hopefully nothing new there.

However, for a 5 dof machine, I would expect to see gcode that sets the orientation of cutter axis 1st, and hence the orientation of x/yplane.  z would always be parallel to the cutter axis and  x/y would always be orthogonal to the spindle axis, no matter which orientation the cutter assumes.  If that's truly the case (and I'm making an assumption here) , then as long as the code in the Mxxx macro is incremental (or at least appropriate to the 5 dof system), then the posted code substitution method should be universal, and no maths/ or calculations should be needed.  It ought to just work.

Peter

[ryan]

You're right I do have a 5 axis machine and I actually think you're work around should function well for me (still probably test in air ;)...however, I would venture to say that a large portion of the shops using the lamello system on a cnc, are running aggregate heads. 

What I would be concerned about is guys running highly customized post-processors to properly position their aggregate heads where an incremental move might not produce the expected result depending on how the post has been modified to accommodate the aggregate. This is beyond my depth though, maybe someone with experience programming aggregates can comment on how planes are defined by a post in this application and whether incremental moves would behave the same.

[daniel_lyall]

I know someone who edited a post for aggregate heads it was not easy and used a lot of fancy math to get it done, I would say that's why most get a plugin done or do it by hand.