zig zag profile tool path

This forum is for general discussion regarding VCarve Pro
Post Reply
cusoak
Vectric Wizard
Posts: 486
Joined: Mon Nov 06, 2017 1:57 pm
Model of CNC Machine: Shapeoko 3D XXL

zig zag profile tool path

Post by cusoak »

New Cabinet side drawer slots.crv
(30 KiB) Downloaded 55 times
I am building a parts cabinet It is going to have drawers in it thw the bottom will be larger than the box itself by .25 on both sides.
The bottom will fit into slots in the cabinet sides
Attached is a file that i have laid out with vectors to make the profile cut on the line to create the groves for the bottoms to fit into.
What I want to happen is that the bit will start out side moving in to the material 1 pass then stop plunge down to the final depth and come back to the original start position move up and do the same thing to all of the rest of the vectors.
Eliminating excess movement.
But I have tried different thing to no avail
Can this even be done.
Thanks Jeff

User avatar
Adrian
Vectric Archimage
Posts: 14544
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: zig zag profile tool path

Post by Adrian »

There are a few things you can do to make it more efficient. Spiral ramps or a vector that goes back along itself will reduce the number of pass retracts. Alternate the start points on the vectors so the next one down starts where the previous one ends.

4DThinker
Vectric Wizard
Posts: 1701
Joined: Sun Sep 23, 2012 12:14 pm
Model of CNC Machine: CNC Shark Pro, Probotix Meteor 25" x 50"

Re: zig zag profile tool path

Post by 4DThinker »

No, and yes. The yes version just requires adding more vectors to tell the bit specifically what to do. The fluting toolpath can be set to go back and forth, stepping down as you wish. It requires a centerline to follow though. Make an offset line by 1/2 the diameter of the endmill you want to use, then use the fluting toolpath on that line. Choose ramp at start, but set the ramp to a small value such as .001". Ramp type linear. The toolpath created will step down the pass depth you have set for the bit you are using, and go back and forth to get to the cut depth you set.
Fluting to profile cut 4D.crv3d
(26.5 KiB) Downloaded 47 times
Fluting to profile cut 4D.crv
(18 KiB) Downloaded 43 times
4D

cusoak
Vectric Wizard
Posts: 486
Joined: Mon Nov 06, 2017 1:57 pm
Model of CNC Machine: Shapeoko 3D XXL

Re: zig zag profile tool path

Post by cusoak »

how are the two files posted different.
Thanks for the help

User avatar
martin54
Vectric Archimage
Posts: 7339
Joined: Fri Nov 09, 2012 2:12 pm
Model of CNC Machine: Gerber 48, Triac PC, Isel fixed gantry
Location: Kirkcaldy, Scotland

Re: zig zag profile tool path

Post by martin54 »

cusoak wrote:
Tue Mar 17, 2020 11:54 pm
how are the two files posted different.
Thanks for the help
I haven't looked but they probably aren't different, one is an Aspire File & the other is a Vcarve file if you look at the file extension :lol: :lol:

4DThinker
Vectric Wizard
Posts: 1701
Joined: Sun Sep 23, 2012 12:14 pm
Model of CNC Machine: CNC Shark Pro, Probotix Meteor 25" x 50"

Re: zig zag profile tool path

Post by 4DThinker »

cusoak wrote:
Tue Mar 17, 2020 11:54 pm
how are the two files posted different.
Thanks for the help
When making a post, down at the bottom is a tab for attachments. Click on it and you'll see a button to click to add files.
If you meant to ask "why" rather than "how", then I use Aspire but posted both versions so those using VCarve or Aspire could download and use them directly. A few seconds of wasted time that didn't hurt because Aspire can also open .CRV file directly.

4D

cusoak
Vectric Wizard
Posts: 486
Joined: Mon Nov 06, 2017 1:57 pm
Model of CNC Machine: Shapeoko 3D XXL

Re: zig zag profile tool path

Post by cusoak »

I guess maybe I did not make myself clear.
I want to lay out and cut 6 .25 wide dados 8 inches long and .25 inches deep in a piece of material that is .75 thick. using a .25 end mil.
I would like the tool to make 1 pass at .125 goto the end of the vector then plunge down to .25 and come back to the start point and then move up to the next vector and do the same thing until it has done all 6 rows not cut
4d thinker I did not want to cut all the way through the wood.
Jeff

User avatar
Adrian
Vectric Archimage
Posts: 14544
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: zig zag profile tool path

Post by Adrian »

They're just examples of techniques that you can use. I suggested a few as well.

You need to experiment with those techniques to see what works for you and understand the methods.

If you want someone to do the actual work for you then that's a different thing from people guiding you towards the tools you need to learn how to do it yourself.

cusoak
Vectric Wizard
Posts: 486
Joined: Mon Nov 06, 2017 1:57 pm
Model of CNC Machine: Shapeoko 3D XXL

Re: zig zag profile tool path

Post by cusoak »

I have never asked anyone to do a file for me.
If you all got that impression then I am sorry.
That was and is not my intention.
when I post here
Jeff

User avatar
TReischl
Vectric Wizard
Posts: 4584
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 48X36X7 RP 2022 UCCNC Screenset
Location: Leland NC

Re: zig zag profile tool path

Post by TReischl »

Surprising sometimes how a simple thing can turn out to be a real challenge.

And yup, this is a simple thing. Forget six dadoes. Just think about one.

Move to position for start.
Plunge cut to first depth
Mill dado
Plunge to second depth
Mill back to start point
Retract

Wash rinse repeat.

The only way I see to do it is by manual coding unless extra moves or double trips are ok.

G0X start Y start
G0Z safe position above work
G1Z-.125Fwhatever
G1X end point (or Y end point) Fwhatever
G1Z-.25Fwhatever
G1X start point (or Y start point)Fwhatever
G0Z safe position above work.

Vectric software is not full 3 axis programming software in that it cannot read 3 axis vectors and cut them. For instance, a vector described as: X0Y0Z1 - X2Y2Z0 cannot be read by the software. As others have posted about above there are some things that you can do to sort of do 3 axis work but in reality those are just workarounds or "tricks".

If you really have to do it this way and not just because it would be nice to do then I would insert that code above into the rest of the program at an appropriate location and get on with it. If it is not something critical then I would just use one of the techniques explained above and get on with it.
"If you see a good fight, get in it." Dr. Vernon Johns

4DThinker
Vectric Wizard
Posts: 1701
Joined: Sun Sep 23, 2012 12:14 pm
Model of CNC Machine: CNC Shark Pro, Probotix Meteor 25" x 50"

Re: zig zag profile tool path

Post by 4DThinker »

cusoak wrote:
Wed Mar 18, 2020 1:50 pm
I want to lay out and cut 6 .25 wide dados 8 inches long and .25 inches deep in a piece of material that is .75 thick. using a .25 end mil.
I would like the tool to make 1 pass at .125 goto the end of the vector then plunge down to .25 and come back to the start point and then move up to the next vector and do the same thing until it has done all 6 rows not cut
4d thinker I did not want to cut all the way through the wood.
Jeff
Put a centerline down the center of where you want the dados.
Select all the centerlines.
Choose the vcarve toolpath.
Set the flute depth to .25".
Choose a 1/4" end mill, and make sure it has a pass depth of .125".
Choose Ramp at Start.
Select ramp Length, and enter 0.001 inches.
Select Ramp Type: Linear.
Click on calculate.

I would have just used the file you posted, but I don't have version 10.
Six 8 inch dados.crv
1/4 inch deep, 2 passes .125 each
(16.5 KiB) Downloaded 48 times
Six 8 inch dados.jpg
4D

User avatar
TReischl
Vectric Wizard
Posts: 4584
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 48X36X7 RP 2022 UCCNC Screenset
Location: Leland NC

Re: zig zag profile tool path

Post by TReischl »

That is pretty darn good 4D!

In the code generated only one "extra move" that I could see:

N80X0.0000Y0.0000F100.0 'Start at 0,0
N90G00X-2.1976Y-3.5062Z0.2500 'Position for first cut
N100G00Z0.1000 'Rapid to .1 above material
N110G1Z-0.1250F30.0 'Feed to .125 cut depth 1 st cut
N120G1X0.4641F100.0 'Cut along X
N130G1X0.4651Z0.0000 'Retract to Z0 at feedrate
N140G1X0.4641Z-0.2500 'Cut to second depth
N150G1X-2.1976 'Cut to initial start position
N160G00Z0.2500
N170G00Z1.2500
N180G00X0.0000Y0.0000

If'n it were me, that would be plenty good!
"If you see a good fight, get in it." Dr. Vernon Johns

User avatar
adze_cnc
Vectric Wizard
Posts: 4325
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: zig zag profile tool path

Post by adze_cnc »

Ramp length could be 0 so your machine doesn't have to do a Z move with 1/1000" X-offset.

4DThinker
Vectric Wizard
Posts: 1701
Joined: Sun Sep 23, 2012 12:14 pm
Model of CNC Machine: CNC Shark Pro, Probotix Meteor 25" x 50"

Re: zig zag profile tool path

Post by 4DThinker »

TReischl wrote:
Wed Mar 18, 2020 8:45 pm
That is pretty darn good 4D!

In the code generated only one "extra move" that I could see:
N130G1X0.4651Z0.0000 'Retract to Z0 at feedrate
Yep. Where it lifts up is the start point of the vectors, and that is where the ramp starts even though the ramp length is effectively zero. Give me a little while and I may figure out a way to eliminate that extra 1/4" of Z travel on each vector.
merged profiles on the line 4D.crv
(34.5 KiB) Downloaded 33 times
Using merge on two profile toolpaths, with one set to Climb and the other to Conventional, optimized for bottom to top, and shortest path, ends up looking like there is no wasted Z lift between passes, but it is impossible to tell for sure just looking at the render play slowly.
4D

cusoak
Vectric Wizard
Posts: 486
Joined: Mon Nov 06, 2017 1:57 pm
Model of CNC Machine: Shapeoko 3D XXL

Re: zig zag profile tool path

Post by cusoak »

I want to Thank 4D for your help. The Fluting Tool Path Does just what I was looking for
Thanks Jeff

Post Reply