Profile Cut using wrong reference with V11.506

[TomWS]

I updated VCarve Pro today to 11.506 from 11.504 and I am now having a very odd behavior. Maybe the earlier version did this and I hadn't noticed or it's a result of the update. But here goes:

I have a 3D model (.OBJ) that I've been working with and found that I really want a clearance profile to provide room for the deep plunge in the 3D Finish profile. So I added a profile toolpath and got this:

I then realized I was cutting through the tabs so I checked 'Project Toolpath onto 3D Model and then I got this, where the starting cut is well below the surface and it cuts all the way through the material.

What I want is the profile cut to start at the top surface of the material and just cut 23mm deep but avoiding the tabs I added to the 3D model. How do I fix this???

[SteveNelson46]

Add a level for manual tabs and for a zero plane and for the model. Three levels total. Add manual tabs then toolpath the model using the level instead of a vector.

[TomWS]

Sorry, I'm not following you. Level isn't a choice with the Profile Tool path. Here are my components (I did add a Zero Plane but it didn't have any effect) and my Material settings.

[SteveNelson46]

There are a lot of factors here to use this technique. A level is part of the Vectric setup on the modeling tab. I'm assuming that you already have the model of the spoon. As shown in the pic, put your model in the component level and the manual tabs in the tabs level. Manual tabs can be added from the clipart tab. Also put the zero plane in the limit plane level. Be sure to resize the tabs and place them in places that won't interfere with the model.

There is a good Vectric training video of the "Two sided Marlin" that shows this technique.

https://www.vectric.com/support/tutoria ... ded-marlin

Another way to do this for just a one sided project is to set the thickness of the model to less than the thickness of the material. Then a normal cutout or profile toolpath with tabs will work. It just depends on how you want to do it and how you want the finished project to look.

[TomWS]

A level is part of the Vectric setup on the modeling tab. I'm assuming that you already have the model of the spoon. As shown in the pic, put your model in the component level and the manual tabs in the tabs level. Manual tabs can be added from the clipart tab. Also put the zero plane in the limit plane level. Be sure to resize the tabs and place them in places that won't interfere with the model.

Yes, I've done all that, as I show in the previous photo, except for putting the Zero plane in the Limit Planes component, but, even after I do that, the profile start cut is too deep.

[SteveNelson46]

With the component and the material the same thickness you don't need a profile or cutout tooloath

[TomWS]

With the component and the material the same thickness you don't need a profile or cutout tooloath

True if the component is uniform thickness as with your example. However, looking at the side view of this project, you can see the range of depth from both sides is fairly large.

[SteveNelson46]

This technique is usually used for 2-sided projects where the tabs can be positioned in the same location on both sides as shown in the Marlin video. It will work for single sided projects also if the material and the model are the same thickness. Otherwise, a regular cutout profile toolpath using system placed tabs is all that is necessary.

[SteveNelson46]

Can you post your project? If it too big to post you can use an external storage location like Google Drive, One drive or Dropbox. You can also send me a private message and I can send you my email address.

[adze_cnc]

I expect you have a vector that represents the border of the entire spoon. You might try this:

• leave the existing border intact but copy it to a new layer (I'm going to call that layer: relief)
• change to the relief layer
• split the border vector on the relief layer into two pieces on each side of the centre line where the handle meets the bowl (you may need to add nodes)
• create two profile toolpaths
  1. one for the bowl vector using whatever depth you think is good (vertical centre of the 3D tab?)
  2. one for the bowl vector using whatever depth you think is good (it will be shallower than the bowl)
• for each of those two toolpaths set the it to cut "outside the line". You may have to alter the starting point of the vector to get it right
• for each of those two toolpaths add tabs centred on the 3D tabs as wide and thick as you want those tabs to be

[TomWS]

@ adze_cnc, that sounds like a good workaround, thanks.

However, Is the behavior I'm seeing 'normal'? If I don't 'project' then the profile is what I expected, starting at the surface, but if I project, expecting the 3D Tabs to be avoided, then the depth of cut shifts completely.

[adze_cnc]

Project to 3D says start the cut at the level of the 3D model. Since you are cutting outside the spoon the "3D model" is the zero plane at the bottom of the material. It behaves properly with the tabs because they are outside the spoon and have their own z position.

The problem with using the project to 3D option is that program presumes there is not material above that model. Thus you could be trying to slam the bit through a great amount of real material to get to the 3D model top.

[TomWS]

Ah, ok, thank you for the explanation. I now understand what is happening. That I noticed is just when I had upgraded made me nervous that the upgrade wasn't good. So, this 'solves' my problem. Back to the drawing board tomorrow!

[SteveNelson46]

I responded to your PM but here is a repeat.
I only have Aspire so I can't post a .crv file with components. Here are the instructions I used.

First, it would be better to use a material thickness of 25mm instead of 35mm. Your model thickness is only 21.192mm. But, if that's all you have it's okay

Top
Set the depth of the limit plane on the top to -.2mm using the properties
Delete the profile toolpath
You really don't need the second bit in the 3D toolpath. Just the 1/8" tbn will do the job and will reduce the cut time considerably.
In the 3D toolpath setup, set the Machining Limit Boundary to use a level and select the "Model" level. Also set the boundary offset to 3mm. That will allow an overcut and eliminate the need for a profile cutout. By selecting to use a level in the Machining Limit Boundary, the toolpath will skip over the tabs as long as they are on a different level.
Back
You can delete the limit plane on the back side.
On the 3D toolpath setup do the same as the top. Delete the 1/4" bit, set the Machining Boundary Limit to use the "Model" level and set the boundary offset to 3mm
Make sure the project is set to the middle of the board.

Let me know if I missed anything

[TomWS]

Thanks! I'll look at it later today, FWIW, the model was supposed to be thicker, not sure why it's as flat as it is...