3D Finishing Toolpaths

This section is for useful tips and tricks for Aspire
Post Reply
BassCentral
Posts: 12
Joined: Wed Jan 27, 2021 6:48 am
Model of CNC Machine: Shark HD5

3D Finishing Toolpaths

Post by BassCentral »

Greetings Vectric forum:
I'm relatively new to Aspire but nonetheless took on a pretty ambitious two-sided, 3D project for my first go. I have designed a bass guitar neck using the two-rail sweep modeling technique described in the Vectric Tips and Tricks video "Making a Guitar Neck." The design took 6 months for me to complete, but I like the final product. This weekend I loaded up my material on the Shark HD5 and ran the roughing toolpaths successfully. I then ran the finishing toolpaths (2 tiles) on one side and it also came out flawlessly. On the other side, I got through about 90% of a 90-minute finishing toolpath and was just finishing out the perimeter of the model. Then, for whatever reason, the machine suddenly jammed the 1/8" ball nose straight through the full thickness of the material (about 0.60") and attempted to cut at full speed. As you might imaging, this quickly broke my $60 Amana tool. This seems to be a problem (a flaw in the software?) that does not limit the maximum depth of cut on the finishing toolpath. Does anyone know how I might force such a limitaiton on the toolpath? For the finishing toolpath, my machining limit boundary is set to "Selected Vector(s)," and I am using a boundary offset of 0.125". I am using the "Offset" area machine strategy with a "Conventional" cut direction.

Any help you can offer would be greatly appreciated. I'm afraid to re-attempt this toolpath and may end up cutting the rest out by hand unless I can come up with a solution.

Thank you!

Scott Winslow
Long Beach, CA

Charlie_l
Vectric Craftsman
Posts: 105
Joined: Sat Jun 30, 2012 1:41 am
Model of CNC Machine: CAMaster Stinger II
Location: Wisconsin

Re: 3D Finishing Toolpaths

Post by Charlie_l »

That is a real disappointment I’m sure.

If you are able I would open the machine code file (Gcode?) to figure out if the z actually went lower just as instructed, or if you had a mechanical glitch. You can also look at your Aspire preview closely to see if there is a low z hole where it dove into your material.
Charlie
Aspire, CAMaster Stinger II

User avatar
Adrian
Vectric Archimage
Posts: 11928
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: 3D Finishing Toolpaths

Post by Adrian »

BassCentral wrote:
Mon Mar 01, 2021 5:01 am
This seems to be a problem (a flaw in the software?) that does not limit the maximum depth of cut on the finishing toolpath. Does anyone know how I might force such a limitaiton on the toolpath? For the finishing toolpath, my machining limit boundary is set to "Selected Vector(s)," and I am using a boundary offset of 0.125". I am using the "Offset" area machine strategy with a "Conventional" cut direction.
It's not a flaw in the software. It is documented that the finishing toolpath is always cut in a single pass and the cut depth is ignored. That's why it's important to make sure that the roughing toolpath is removing sufficient material.

This is the actual text from the Help regarding it:
finish.jpg

User avatar
mtylerfl
Vectric Archimage
Posts: 5486
Joined: Thu Jan 29, 2009 3:54 am
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha
Location: Brunswick, GA
Contact:

Re: 3D Finishing Toolpaths

Post by mtylerfl »

Hi Scott,

Sorry to hear about your broken bit!

If you are willing, please upload your file to DropBox (or similar free service), and post the download link here. Some of us can take a close look at your file layout and Toolpaths to see if we can spot exactly where the massive plunge occurred and how to prevent it (perhaps with merged limit planes or whatever).

If nothing appears unusual or out of order in your file, then at least you can rule that out and focus on possible machine issues, etc.
Michael Tyler

carvebuddy.com

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC

User avatar
adze_cnc
Vectric Apprentice
Posts: 1645
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: 3D Finishing Toolpaths

Post by adze_cnc »

BassCentral wrote:
Mon Mar 01, 2021 5:01 am
Then, for whatever reason, the machine suddenly jammed the 1/8" ball nose straight through the full thickness of the material (about 0.60") and attempted to cut at full speed. ... For the finishing toolpath, my machining limit boundary is set to "Selected Vector(s)," and I am using a boundary offset of 0.125".
The centre of the the 1/8" bit was moved 1/8" away from the the model effectively making it cut "not on the model".

For situations like this, besides running 3D Roughing toolpath I will run a 2D profile "relief" cut. The cut depth will be material thickness minus a reasonable amount (probably 1/8 inch—so, in your case a depth of 0.475"). This gives the finishing bit room to plunge to full depth if it needs to.

BassCentral
Posts: 12
Joined: Wed Jan 27, 2021 6:48 am
Model of CNC Machine: Shark HD5

Re: 3D Finishing Toolpaths

Post by BassCentral »

Thank you all so much for your quick response. Adrian's reply confirmed my previous thought that maximum cut depth cannot be set for the finishing toolpath. Adrian, I did set the roughing toolpath to only leave 0.20" material for the finishing toolpath to remove. This is why I was surprised that it decided to go for a >0.5" cut on that last pass.

I was just looking at the most recent input from Vectric Apprentice, and his assessment seems very logical. What seems to be happening is my finishing bit is effectively "falling off the edge" of my model, thereby losing any reference it previously had for assigning the cut depth. Seems to me I have read something about this before. Apprentice's solution also seems feasible. Apprentice, if I understand your tip correctly, I should create a new 2D profile toolpath (depth = material thickness minus 1/8") and instruct the tool to remain outside of the selected vector (i.e., the neck perimeter). Then, in sequence, run my existing roughing toolpath first, then the 2D profile ("relief") cut, then my existing finishing toolpath. Perhaps a side benefit to this workflow would be to create a smoother edge since this is being defined largely by a 2D toolpath rather than a 3D one which tends to leave a "rasterized" edge.

User avatar
adze_cnc
Vectric Apprentice
Posts: 1645
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: 3D Finishing Toolpaths

Post by adze_cnc »

A little pictorial essay.

Steven
Boot-last with roughing pass
Boot-last with roughing pass
Added profile relief pass (material thickness minus 1/4") that doubles as preliminary cut-out pass for the vertical boot bottom
Added profile relief pass (material thickness minus 1/4") that doubles as preliminary cut-out pass for the vertical boot bottom
3D finish pass has room for the bit to plunge 2.25" deep in spots without crashing
3D finish pass has room for the bit to plunge 2.25" deep in spots without crashing
Profile pass to trim up the final 1/4"
Profile pass to trim up the final 1/4"

BassCentral
Posts: 12
Joined: Wed Jan 27, 2021 6:48 am
Model of CNC Machine: Shark HD5

Re: 3D Finishing Toolpaths

Post by BassCentral »

Hi Steven:
I just finally got a chance to take a close look at your post. Very nice of you to provide the pictorial essay. I recieved my replacement tools from ToolsToday this afternoon and am ready to give it another shot. Once thing that will make my job a bit more tricky than your essay is that mine is a two-sided carving. Not exactly sure how I would approach the relief cuts in a way that doesn't cut completely through the model in some areas.

Scott

BassCentral
Posts: 12
Joined: Wed Jan 27, 2021 6:48 am
Model of CNC Machine: Shark HD5

Re: 3D Finishing Toolpaths

Post by BassCentral »

Here's another possible workflow that might be a solution to the tool-snapping problem:

1) Revise the 3D finishing toolpath by changing the machining limit boundary offset from the full tool diamter (0.125") to 0" and recalculate. This would be done for both sides of the job. In theory, I would think that this would force the outermost finishing pass to remain within the boundaries of the model and not "fall off the edge" and cause a full depth plunge that would snap the tool (again).
2) Run the 3D roughing toolpath as currently written on both sides of the model.
3) Run the newly recalculated 3D finishing toolpath on both sides of the model. I just ran the preview for this, and it now shows no deep plunges through the model.
4) Create a new 2D profile toolpath that is set up to run along the outside perimeter of the guitar neck vector. This could be done with a 1/4" end mill with a sufficient length to fully penetrate the model thickness. In order to avoid cutting through the 3D tabs, I would also create 2D tabs in the profile toolpath that coincide with the positions of the 3D tabs.
5) As a final step, run the profile toolpath and, hopefully, achieve a nice, smooth perimeter cut.

Does this sound like a feasible solution, or am I just showcasing my inexperience?

Thank you all for your input.

Scott

Post Reply