First 3D Project - Noob Problems

This forum is for general discussion regarding VCarve Pro
halodri
Vectric Apprentice
Posts: 55
Joined: Tue Jul 26, 2022 11:42 am
Model of CNC Machine: BZT PFK 1607 PX

Re: First 3D Project - Noob Problems

Post by halodri »

Adrian wrote:
Wed Mar 01, 2023 10:56 am
If you define the material as 8' x 4' and then import a model that is 10" x 6" the vast majority of the pixels available are wasted in blank space.
Ok, this is also good to know, thanks!

halodri
Vectric Apprentice
Posts: 55
Joined: Tue Jul 26, 2022 11:42 am
Model of CNC Machine: BZT PFK 1607 PX

Re: First 3D Project - Noob Problems

Post by halodri »

Is it possible/advised to do a roughing toolpath before doing a 45° chamfer toolpath?
Attachments
Capture.JPG
61jG1jAy5+L._SL1000_.jpg

halodri
Vectric Apprentice
Posts: 55
Joined: Tue Jul 26, 2022 11:42 am
Model of CNC Machine: BZT PFK 1607 PX

Re: First 3D Project - Noob Problems

Post by halodri »

Is this a good (the only?) procedure? :

1. Create a 3D roughing toolpath based on a 3D model.

2.Run a 45° chamfer toolpath based on a 2D vector.

User avatar
Adrian
Vectric Archimage
Posts: 14546
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: First 3D Project - Noob Problems

Post by Adrian »

Don't see any need to run a separate toolpath for the Chamfer toolpath. The 3D roughing toolpath is designed to be used with the 3D finish toolpath.

If you're concerned about how big a "bite" the Chamfer toolpath is taking then reduce the pass depth of the tool to create more passes.

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: First 3D Project - Noob Problems

Post by martin54 »

Every project is different so when you are combining 2D & 3D toolpaths then you need to look closely at what you are doing, in this example then I wouldn't run the 3D roughing toolpath first as from what I can see there is no need, I would simply run the 2D chamfer toolpath which is firstly likely to take less time & will give me a better finish overall.
As Adrian has said if the V bit is cutting to deeply on each pass then alter the cut depth for the V bit. You can either do this in the tool database which will result in a permanent change to the V bit cut depth or you can alter it within the chamfer toolpath by clicking on the edit button & changing it there which will only alter it for that one toolpath :lol: :lol:
cham.jpg

halodri
Vectric Apprentice
Posts: 55
Joined: Tue Jul 26, 2022 11:42 am
Model of CNC Machine: BZT PFK 1607 PX

Re: First 3D Project - Noob Problems

Post by halodri »

Adrian wrote:
Fri Mar 03, 2023 12:01 pm
...don't see any need to run a separate toolpath

If you're concerned about how big a "bite" the Chamfer toolpath is taking then reduce the pass depth of the tool to create more passes.
martin54 wrote:
Fri Mar 03, 2023 2:40 pm
I wouldn't run the 3D roughing toolpath first as from what I can see there is no need, I would simply run the 2D chamfer toolpath which is firstly likely to take less time & will give me a better finish overall.
cham.jpg

Right, I was concerned it might be "to big of a bite" but I have no experience so my concerns are not really valid. Thank you for your answers, I'll follow your recommendation and use a chamfer toolpath only.

What would be a reasonably path depth?

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: First 3D Project - Noob Problems

Post by martin54 »

What would be a reasonably path depth?

That kind of depends on your machine & how it is set up, what works well for me might be either to much for your set up or you might find you can cut deeper than I do, experiment a bit yourself BUT be aware that because the bit is V shaped the deeper the bit actually cuts the more of the cutting edge is going to be engaged which will increase the load on the machine :lol: :lol:

User avatar
adze_cnc
Vectric Wizard
Posts: 4329
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: First 3D Project - Noob Problems

Post by adze_cnc »

You might also want to use the “Edit passes…” button to make asymmetric pass depths.

If you are cutting 12mm deep and your tool’s pass depth is 3mm you’ll get 4 passes each of 3mm. But the first one or maybe two passes will have very little V engagement and the last two will have much more. You could manually change the passes so that they are something like:
  • 4.5mm
  • 3.5mm
  • 2.5mm
  • 1.5mm
or some other descending combination.

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: First 3D Project - Noob Problems

Post by martin54 »

adze_cnc wrote:
Sat Mar 04, 2023 4:29 pm
You might also want to use the “Edit passes…” button to make asymmetric pass depths.

If you are cutting 12mm deep and your tool’s pass depth is 3mm you’ll get 4 passes each of 3mm. But the first one or maybe two passes will have very little V engagement and the last two will have much more. You could manually change the passes so that they are something like:
  • 4.5mm
  • 3.5mm
  • 2.5mm
  • 1.5mm
or some other descending combination.
The chamfer toolpath won't let you edit the passes in the same way some of the other toolpaths do, could be a good feature request :lol: :lol:

User avatar
SteveNelson46
Vectric Wizard
Posts: 2282
Joined: Wed Jan 04, 2012 2:43 pm
Model of CNC Machine: Camaster Stinger 1
Location: Tucson, Az.

Re: First 3D Project - Noob Problems

Post by SteveNelson46 »

I must have missed something. As far as I can see, this is just a simple 2D project using the moulding toolpath.
Attachments
Cutting board.png
Cutting board setup.png
Cutting board.crv
(570 KiB) Downloaded 13 times
Steve

halodri
Vectric Apprentice
Posts: 55
Joined: Tue Jul 26, 2022 11:42 am
Model of CNC Machine: BZT PFK 1607 PX

Re: First 3D Project - Noob Problems

Post by halodri »

martin54 wrote:
Sat Mar 04, 2023 2:46 pm
... because the bit is V shaped the deeper the bit actually cuts the more of the cutting edge is going to be engaged which will increase the load on the machine :lol: :lol:
Yep, the thought has occurred to me too. Yesterday I did a test piece and I first used a profile toolpath to cut out the perimeter and removed it before doing the chmafer toolpath so that the V-bit does not have to dive into the full material.
Capture.JPG
2.JPG
adze_cnc wrote:
Sat Mar 04, 2023 4:29 pm
You might also want to use the “Edit passes…” button to make asymmetric pass depths.
I use " Edit passes" quite a bit for flat end mills. I just checked the "edit passes" for the V-bit, but as Martin mentioned, the chamfer toolpath doesn't have this functionality.
SteveNelson46 wrote:
Sun Mar 05, 2023 2:09 am
I must have missed something. As far as I can see, this is just a simple 2D project using the moulding toolpath
You are perfectly right. This turned out to be just a 2D project. I might make another test piece with rounded screw hole edges to make it 3D.



As I didn't know which cutting parameters to use for the V-bit, I just used the cutting parameter for the 8mm end mill that cut out the perimeter, but with a path depth of 2mm. During the maching I bumbed up the feedrate to 200% to speed up the process.
1.JPG
The end result wasn't too bad, except fo stronge cutting marks at the top caused by wobbling due to insufficient securing of the piece with screws (and that one of the screw heads broke off). However, I'm a bit bothered by the noticeable tear out in two of the diagonal corners. I'm not sure if a slower feed rate would reduce tear out, as it may also depend on the wood species and simply the nature of round corners. I used glue-laminated beech wood, 38mm thick. I guess the only post processing step is to fill the tear out with saw dust but that doesn't look pretty.
Attachments
IMG_20230305_090144.jpg
IMG_20230305_090204.jpg
IMG_20230305_090216.jpg

halodri
Vectric Apprentice
Posts: 55
Joined: Tue Jul 26, 2022 11:42 am
Model of CNC Machine: BZT PFK 1607 PX

Re: First 3D Project - Noob Problems

Post by halodri »

I made a second piece, and it turned out much better with almost no tear-out (except for too shallow holes). I significantly increased the RPM to 24,000 and lowered the feed rate. I also believe that the larger radius helped. I'm not sure if this is optimal, but it worked for my purpose.
Attachments
IMG_20230306_104035.jpg

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: First 3D Project - Noob Problems

Post by martin54 »

your spindle speed is probably to high at 24000 especially if you have also reduced the feedrate but an easy check is to feel the cutting bit the minute the has stopped after cutting, if the bit is hot to the touch then you are creating a lot of friction which isn't good for tool life :lol: :lol:

You can also do this without making a complete new part by using the offset function or creating a new vector outside of the original chamfer tool vector, use that for some testing & then once you are happy use the original vector or remove the offset for the final cut :lol: :lol:

halodri
Vectric Apprentice
Posts: 55
Joined: Tue Jul 26, 2022 11:42 am
Model of CNC Machine: BZT PFK 1607 PX

Re: First 3D Project - Noob Problems

Post by halodri »

martin54 wrote:
Mon Mar 06, 2023 2:06 pm
... but an easy check is to feel the cutting bit the minute the has stopped after cutting, if the bit is hot to the touch then you are creating a lot of friction
Interesting, because I have done that and was surprised to find the bit only lukewarm. I am glad to read that this is an approved method. :D However. I am sure by conventional wisdom, the RPM was much too high. In my understanding this can shorten tool life and cause burn marks. My current thinking is that if a too high RPM can fix tear-out, with the cost of shortening tool life that is an acceptable trade-off, since the bit is rather cheap.
martin54 wrote:
Mon Mar 06, 2023 2:06 pm
You can also do this without making a complete new part by using the offset function or creating a new vector outside of the original chamfer tool vector, use that for some testing & then once you are happy use the original vector or remove the offset for the final cut :lol: :lol:
Right, that's a good way to check if the settings are appropriate. I'll keep that in mind.

Sjirk
Posts: 6
Joined: Thu Mar 16, 2023 3:38 pm
Model of CNC Machine: DAMEN CNC

Re: First 3D Project - Noob Problems

Post by Sjirk »

Hello everybody. I do not know if my questions can be asked in this item but i give it a try. What i want to do is make a rectangular hole in a material with a round top cutter, let's say diameter 8, radius 4. All the lines will have a 4mm radius. BUT i want the corners to heve a bigger radius, let's say 10mm radius. Is that possible? How do i round of corners in all 3 dimensions? Hope i made myself clear enough. Thanks!

Post Reply