Reversing toolpath

This forum is for general discussion regarding VCarve Pro
User avatar
badgersurfer
Posts: 44
Joined: Sun Jul 24, 2016 12:24 pm
Model of CNC Machine: xcarve

Reversing toolpath

Post by badgersurfer »

I am sure this has been asked a thousand times but I cannot find it anywhere. I am currently making jigs and I simply have a straight toolpath about 70mm long. I is a 3mm tool and is cutting a 3mm slot 10 mm deep and 1mm each pass. When it cuts it goes from the start point to the end of the path then lifts and traverses back to the start point for the next cut. Is there a simple way of making it cut in both directions as it takes a long time keep returning to the start point.

kzeyus
Vectric Wizard
Posts: 346
Joined: Wed Sep 27, 2006 4:05 pm
Location: Rogers, AR

Re: Reversing toolpath

Post by kzeyus »

Snap1.jpg
If I understand what you are asking, and assuming your are doing a profile 'on' the vector, just connect the vectors beyond the edge of the material. Easiest to do if you reverse the start point of every other vector then join with the 'join with straight line' or 'Join with smooth curve' tools.
Ken Zey
Rogers, AR
http://www.CedarSlabSigns.com
http://www.lookoutmercantile.com
Shopbot PRS Alpha 72x144

kzeyus
Vectric Wizard
Posts: 346
Joined: Wed Sep 27, 2006 4:05 pm
Location: Rogers, AR

Re: Reversing toolpath

Post by kzeyus »

On second reading, it sounds like you are making 10 passes of 1mm each in the same location. You might try a pocket toolpath where your pocket is just slightly larger than your tool, and set pass depth to 1mm
Ken Zey
Rogers, AR
http://www.CedarSlabSigns.com
http://www.lookoutmercantile.com
Shopbot PRS Alpha 72x144

User avatar
badgersurfer
Posts: 44
Joined: Sun Jul 24, 2016 12:24 pm
Model of CNC Machine: xcarve

Re: Reversing toolpath

Post by badgersurfer »

kzeyus wrote:On second reading, it sounds like you are making 10 passes of 1mm each in the same location. You might try a pocket toolpath where your pocket is just slightly larger than your tool, and set pass depth to 1mm
Yes thanks for that. I have just one straight line going from a to b. I would like it to go (a to b) then (b to a) then (a to b) etc,. dropping 1mm so I would only need to do 5 passes instead of 10x (a to b).

User avatar
Adrian
Vectric Archimage
Posts: 14543
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: Reversing toolpath

Post by Adrian »

Try reversing the vector back on itself so you have a vector that starts and stops in the same place. Basically twice as long folded in half.

tomgardiner
Vectric Wizard
Posts: 447
Joined: Thu Oct 02, 2014 1:49 pm
Model of CNC Machine: FMT Patriot 4 x8

Re: Reversing toolpath

Post by tomgardiner »

I don't think Adrian's suggestion will speed up the cut because the cutter will return to 'a' at feed speed not rapid.
Would using a spiral ramp work? You would setup the depth per pass at 1mm and I think the router will return on the line to full depth the make a single pass full depth. Set your plunge rate to the same as standard feed for this run.

ger21
Vectric Wizard
Posts: 1592
Joined: Sun Sep 16, 2007 2:59 pm
Model of CNC Machine: Custom DIY
Location: Lake St Clair, MI, USA
Contact:

Re: Reversing toolpath

Post by ger21 »

Yes, draw a straight vector, that returns back on itself, so it has 3 points, with the start and end points the same. Use a spiral ramp, and each pass will ramp down, back and forth, to the full depth.
Gerry - http://www.thecncwoodworker.com

User avatar
badgersurfer
Posts: 44
Joined: Sun Jul 24, 2016 12:24 pm
Model of CNC Machine: xcarve

Re: Reversing toolpath

Post by badgersurfer »

ger21 wrote:Yes, draw a straight vector, that returns back on itself, so it has 3 points, with the start and end points the same. Use a spiral ramp, and each pass will ramp down, back and forth, to the full depth.
This idea works, but the only thing I have noticed id that is the same amount of passes 15. I looked at the gcode and it cuts 1 mm in two passes i.e. ramps .5mm (a-b) and then ramps back another .5.. (b-a). I reduced the passes to 7 but then obviously when it comes back towards (a) it is cutting 2mm. Ideally I would like to cut 1mm on each pass then I can half the passes and time. So it would start at (a) move to (b) then plunge 1mm etc.

User avatar
badgersurfer
Posts: 44
Joined: Sun Jul 24, 2016 12:24 pm
Model of CNC Machine: xcarve

Re: Reversing toolpath

Post by badgersurfer »

!!! SUSSED IT !!! ... A 2 minute call to Mark at Vectric and he said it can be done with the fluting tool. An yep a bit of playing around and it is perfect. Here is a picture to explain...Image

tomgardiner
Vectric Wizard
Posts: 447
Joined: Thu Oct 02, 2014 1:49 pm
Model of CNC Machine: FMT Patriot 4 x8

Re: Reversing toolpath

Post by tomgardiner »

Never thought of the fluting path. I am surprised that you have selected the flute in and out option. I would have thought the flute in would be the best option. Remember the feed is determined by the plunge rate when z motions are used.

garylmast
Vectric Wizard
Posts: 1580
Joined: Fri Oct 23, 2009 4:03 pm
Location: Sandy, Utah

Re: Reversing toolpath

Post by garylmast »

If you set the start point on every other vector, it will reverse. Gary
Attachments
Capture.JPG

User avatar
badgersurfer
Posts: 44
Joined: Sun Jul 24, 2016 12:24 pm
Model of CNC Machine: xcarve

Re: Reversing toolpath

Post by badgersurfer »

garylmast wrote:If you set the start point on every other vector, it will reverse. Gary
Not sure what you mean here, I only have 1 line so 1 open vector. It is cutting -z0 to -z15

User avatar
badgersurfer
Posts: 44
Joined: Sun Jul 24, 2016 12:24 pm
Model of CNC Machine: xcarve

Re: Reversing toolpath

Post by badgersurfer »

tomgardiner wrote:Never thought of the fluting path. I am surprised that you have selected the flute in and out option. I would have thought the flute in would be the best option. Remember the feed is determined by the plunge rate when z motions are used.
what do you mean by in and out option?

tomgardiner
Vectric Wizard
Posts: 447
Joined: Thu Oct 02, 2014 1:49 pm
Model of CNC Machine: FMT Patriot 4 x8

Re: Reversing toolpath

Post by tomgardiner »

Sorry, wrong wording. You have selected Ramp at Start and End under Flute Type.(in your screen shot) I would have thought it would be better to Ramp over Complete Length.

User avatar
badgersurfer
Posts: 44
Joined: Sun Jul 24, 2016 12:24 pm
Model of CNC Machine: xcarve

Re: Reversing toolpath

Post by badgersurfer »

tomgardiner wrote:Sorry, wrong wording. You have selected Ramp at Start and End under Flute Type.(in your screen shot) I would have thought it would be better to Ramp over Complete Length.
Yep, Ramp at start is 11 secs faster than the other, but the process seems similar.

Post Reply