Reversing toolpath

This forum is for general discussion regarding VCarve Pro

Reversing toolpath

Postby badgersurfer » Tue Nov 07, 2017 11:29 am

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.
User avatar
badgersurfer
Vectric Apprentice
 
Posts: 23
Joined: Sun Jul 24, 2016 12:24 pm
Model of CNC Machine: xcarve

Re: Reversing toolpath

Postby kzeyus » Tue Nov 07, 2017 1:45 pm

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: 337
Joined: Wed Sep 27, 2006 4:05 pm
Location: Rogers, AR

Re: Reversing toolpath

Postby kzeyus » Tue Nov 07, 2017 1:48 pm

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
kzeyus
Vectric Wizard
 
Posts: 337
Joined: Wed Sep 27, 2006 4:05 pm
Location: Rogers, AR

Re: Reversing toolpath

Postby badgersurfer » Tue Nov 07, 2017 10:10 pm

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
badgersurfer
Vectric Apprentice
 
Posts: 23
Joined: Sun Jul 24, 2016 12:24 pm
Model of CNC Machine: xcarve

Re: Reversing toolpath

Postby Adrian » Wed Nov 08, 2017 9:18 am

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.
User avatar
Adrian
Vectric Archimage
 
Posts: 7422
Joined: Thu Nov 23, 2006 2:19 pm
Location: Surrey, UK
Model of CNC Machine: ShopBot PRS Alpha 96x48

Re: Reversing toolpath

Postby tomgardiner » Wed Nov 08, 2017 1:14 pm

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.
tomgardiner
Vectric Craftsman
 
Posts: 235
Joined: Thu Oct 02, 2014 1:49 pm
Model of CNC Machine: FMT Patriot 4 x8

Re: Reversing toolpath

Postby ger21 » Wed Nov 08, 2017 1:36 pm

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
ger21
Vectric Wizard
 
Posts: 863
Joined: Sun Sep 16, 2007 2:59 pm
Location: Shelby Township, MI, USA

Re: Reversing toolpath

Postby badgersurfer » Thu Nov 09, 2017 11:25 am

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
Vectric Apprentice
 
Posts: 23
Joined: Sun Jul 24, 2016 12:24 pm
Model of CNC Machine: xcarve

Re: Reversing toolpath

Postby badgersurfer » Thu Nov 09, 2017 11:58 am

!!! 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
User avatar
badgersurfer
Vectric Apprentice
 
Posts: 23
Joined: Sun Jul 24, 2016 12:24 pm
Model of CNC Machine: xcarve

Re: Reversing toolpath

Postby tomgardiner » Thu Nov 09, 2017 1:44 pm

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.
tomgardiner
Vectric Craftsman
 
Posts: 235
Joined: Thu Oct 02, 2014 1:49 pm
Model of CNC Machine: FMT Patriot 4 x8

Re: Reversing toolpath

Postby garylmast » Thu Nov 09, 2017 1:57 pm

If you set the start point on every other vector, it will reverse. Gary
Attachments
Capture.JPG
garylmast
Vectric Wizard
 
Posts: 571
Joined: Fri Oct 23, 2009 4:03 pm
Location: Sandy, Utah

Re: Reversing toolpath

Postby badgersurfer » Thu Nov 09, 2017 3:35 pm

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
Vectric Apprentice
 
Posts: 23
Joined: Sun Jul 24, 2016 12:24 pm
Model of CNC Machine: xcarve

Re: Reversing toolpath

Postby badgersurfer » Thu Nov 09, 2017 3:46 pm

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?
User avatar
badgersurfer
Vectric Apprentice
 
Posts: 23
Joined: Sun Jul 24, 2016 12:24 pm
Model of CNC Machine: xcarve

Re: Reversing toolpath

Postby tomgardiner » Thu Nov 09, 2017 5:45 pm

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.
tomgardiner
Vectric Craftsman
 
Posts: 235
Joined: Thu Oct 02, 2014 1:49 pm
Model of CNC Machine: FMT Patriot 4 x8

Re: Reversing toolpath

Postby badgersurfer » Thu Nov 09, 2017 7:13 pm

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.
User avatar
badgersurfer
Vectric Apprentice
 
Posts: 23
Joined: Sun Jul 24, 2016 12:24 pm
Model of CNC Machine: xcarve

Next

Return to VCarve - General

Who is online

Users browsing this forum: Bing [Bot] and 17 guests