Help - Unable to

This forum is for general discussion about Cut3D
Post Reply
User avatar
Bigshew
Posts: 10
Joined: Tue Nov 16, 2021 9:07 pm
Model of CNC Machine: Onefinity
Location: Edmonton, AB, Canada

Help - Unable to

Post by Bigshew »

Hi all. My first post on here.

I have a onefinity and use VCarvePro. I'm trying to cut a 3D design however when the rough cut is complete, I add the 3Dfinish tool ( I used a 1/4 BN) for better detail. That went ok but it seemed to cut a little deeper than it was supposed to. Then when I tried to change the tool for the final detail cut (I used a tapered BN 1/16) it didn't actually seem to zero and then just cut Waaaay too deep at the start of the cut. My design is probably ruined but I need to learn what I'm doing wrong.

I looked here and saw that I should have used a larger piece of wood so that I can zero of the height of the original material height or at least written down the zero height and zeroed from there for Z? When I tried to use my probe, the height of the material was not the same because of the rough cut so I was pretty concerned I had already made a mistake, but I used the probe and the second tool path went ok, but as I said it cut a little deeper than it was probably supposed to. The third toolpath....disaster.

I cant seem to transition between toolpaths smoothly. At times the bit is hard to even change because the machine is so low so I have had to save the toolpaths separately. I need help
Forum.jpeg
https://www.dropbox.com/sh/qe4sspfem0ae ... 6Nyza?dl=0

User avatar
Adrian
Vectric Archimage
Posts: 12404
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: Help - Unable to

Post by Adrian »

When you change a tool you need to set the z-zero at the same level. If you're zeroing off the material surface then that needs to be an area that has not been cut already. If you're zeroing off the table bed then that's not an issue obviously as that doesn't change.

SteveNelson46
Vectric Wizard
Posts: 1449
Joined: Wed Jan 04, 2012 2:43 pm
Model of CNC Machine: Camaster Stinger/WinCNC
Location: Tucson, Az.

Re: Help - Unable to

Post by SteveNelson46 »

For us to look at it you will need to provide the VCarve file itself. Not the toolpath gcode.
Steve

User avatar
adze_cnc
Vectric Apprentice
Posts: 1986
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: Help - Unable to

Post by adze_cnc »

You appear to be zeroing to the material surface so Adrian's comment stands. Also see this recent thread (in particular my first post): viewtopic.php?f=28&t=38690

To save yourself some time—for the roughing, finishing, and rest machining toolpaths—consider using "Selected Vector" instead of "Model Boundary" or "Material Boundary". The Selected Vector would be the same one you are using for the final "Profile Toolpath".

--
2021-11-18_123913.jpg

User avatar
Bigshew
Posts: 10
Joined: Tue Nov 16, 2021 9:07 pm
Model of CNC Machine: Onefinity
Location: Edmonton, AB, Canada

Re: Help - Unable to

Post by Bigshew »

OK thanks everyone. I appreciate you guys confirming that I need to make the material a little bigger than the project. Would it still help if I dropbox the vcarve? or is that really the problem in a nutshell

User avatar
Bigshew
Posts: 10
Joined: Tue Nov 16, 2021 9:07 pm
Model of CNC Machine: Onefinity
Location: Edmonton, AB, Canada

Re: Help - Unable to

Post by Bigshew »

adze_cnc wrote:
Thu Nov 18, 2021 9:40 pm
You appear to be zeroing to the material surface so Adrian's comment stands. Also see this recent thread (in particular my first post): viewtopic.php?f=28&t=38690

To save yourself some time—for the roughing, finishing, and rest machining toolpaths—consider using "Selected Vector" instead of "Model Boundary" or "Material Boundary". The Selected Vector would be the same one you are using for the final "Profile Toolpath".

--
2021-11-18_123913.jpg
I did actually read your post. I think I got a little lost in the process of zeroing of the table or spoilboard or how that works exactly. If I use selected vector instead of Material Boundary, I can just use the probe?

User avatar
adze_cnc
Vectric Apprentice
Posts: 1986
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: Help - Unable to

Post by adze_cnc »

By using the selected vector you've effectively satisfied #1 in my post at the link as the uncut area is the "extra material".

Let's repeat that part of the link above and pretend that we're going to mill away all our material because we're using model boundary instead of selected vector:
  1. before the roughing cut: zero off the table surface
  2. move to the surface of the material
  3. before zeroing to that spot write down the distance we've moved in the Z axis
  4. zero the bit
In number 1 we mark a known location—the spoilboard—and temporarily call it z=0. In #2 we move to the material surface and find that our z co-ordinate is some distance above 0 (let's pretend it is 0.706 inches and as per #3 we write it down for safe keeping). Do #4. Now z=0 is at the surface of the material and the spoilboard is effectively at z = -0.706.

We cut our roughing pass and now have none of the original surface of material left. But we do know two things: 1) where the spoilboard surface is and 2) the distance in the z axis we moved to get to the top of our material (that 0.706 inches).

Now, when you want to zero off the ball-end cutter for the finish passes and the square-end cutter for the profile pass:
  • zero the ball-end (or square-end for profile) to the table surface
  • manually move in the Z axis to the value written down above (in our imaginary case: 0.706)
  • set z-zero to that height
Even though the bit is not touching any material when we set the z-zero in the third step just above we know that it is the actual material surface (before we milled it away) because we verified that in steps 2 & 3 at the top of this post.

User avatar
Bigshew
Posts: 10
Joined: Tue Nov 16, 2021 9:07 pm
Model of CNC Machine: Onefinity
Location: Edmonton, AB, Canada

Re: Help - Unable to

Post by Bigshew »

adze_cnc wrote:
Thu Nov 18, 2021 11:25 pm
By using the selected vector you've effectively satisfied #1 in my post at the link as the uncut area is the "extra material".

Let's repeat that part of the link above and pretend that we're going to mill away all our material because we're using model boundary instead of selected vector:
  1. before the roughing cut: zero off the table surface
  2. move to the surface of the material
  3. before zeroing to that spot write down the distance we've moved in the Z axis
  4. zero the bit
In number 1 we mark a known location—the spoilboard—and temporarily call it z=0. In #2 we move to the material surface and find that our z co-ordinate is some distance above 0 (let's pretend it is 0.706 inches and as per #3 we write it down for safe keeping). Do #4. Now z=0 is at the surface of the material and the spoilboard is effectively at z = -0.706.

We cut our roughing pass and now have none of the original surface of material left. But we do know two things: 1) where the spoilboard surface is and 2) the distance in the z axis we moved to get to the top of our material (that 0.706 inches).

Now, when you want to zero off the ball-end cutter for the finish passes and the square-end cutter for the profile pass:
  • zero the ball-end (or square-end for profile) to the table surface
  • manually move in the Z axis to the value written down above (in our imaginary case: 0.706)
  • set z-zero to that height
Even though the bit is not touching any material when we set the z-zero in the third step just above we know that it is the actual material surface (before we milled it away) because we verified that in steps 2 & 3 at the top of this post.
Thanks a ton! I will try this and let you know if my slow mind can execute haha

Post Reply