full 3d machining to a STL model

[Lumenautica]

Hi all

so I'm having a few issues with machining a part fully using the stl file.

My work flow as standard
generate dxf artwork
create model in fusion
import model with a dxf overlay
3d machine to the dxf boundary then cut the part out ect

here is my issue when I change the boundary offset to allow the finishing tool to travel to the bed along a vertical side of a part or just past the bevel, I'm getting undercuts into the letter. it appears to be related to a resolution or file quality issue. I have tried a few different output options and the stl model still has a pixilated or noisy edge and the tool is following this.

the reason for wanting to machine past the boundary of the bevelled face is to machine the fillet radius where the bevel meets the side so its uniformly machined and requires less sanding.

the bevelled face and details are correct but its just the vertical sides I cant figure out.

How can I over come this?

[Adrian]

You're using a 2mm offset with a 6mm tool. The recommended settings are at least the tool radius to make sure that the tool "drops" fully off the edge as toolpaths are calculated from the centre of the bit.

Vertical edges are always an issue with the Vectric software due to the pixel based nature of the software. The best way around is to use a profile toolpath around the letter itself to clean the edge up.

It's also important to select the correct job resolution when initially creating the job and to ensure the model uses as much of the defined workspace as possible to maximize the number of pixels available. I can see that you've defined the job on an 8x4 sheet so unless that letter is filling the whole sheet most of the pixels are going to waste and reducing the resolution.

Look at the two attached pictures. They are both of a 150mm letter created in standard resolution. The difference is one is on a 200x200 piece of material and the other is on 2440x1220.

[Lumenautica]

You're using a 2mm offset with a 6mm tool. The recommended settings are at least the tool radius to make sure that the tool "drops" fully off the edge as toolpaths are calculated from the centre of the bit.

Vertical edges are always an issue with the Vectric software due to the pixel based nature of the software. The best way around is to use a profile toolpath around the letter itself to clean the edge up.

It's also important to select the correct job resolution when initially creating the job and to ensure the model uses as much of the defined workspace as possible to maximize the number of pixels available. I can see that you've defined the job on an 8x4 sheet so unless that letter is filling the whole sheet most of the pixels are going to waste and reducing the resolution.

Look at the two attached pictures. They are both of a 150mm letter created in standard resolution. The difference is one is on a 200x200 piece of material and the other is on 2440x1220.

Vertical edges are always an issue with the Vectric software due to the pixel based nature of the software. The best way around is to use a profile toolpath around the letter itself to clean the edge up.

This is my standard way of working with this style lettering.

see with the 2mm off set the tool does drop off in places where the stl allows it. (alignment issue?)

re the job resolution that was just a test file please see the attached photos

one thing I've found we create a mutil part stl file to overcome the single file issue.
when I centre this in the job then over lay the dxf and this is centred they do not align so this may be with the tool is dropping one side more than the other. I've tried all manner of settings checking model and dxf sizes all match the alignment seems to all ways be off.

[Adrian]

Rather than using imported DXF's to create vector boundaries you may have better results using the Create Vector Boundary tool in VCarve. That way the boundary is created from the actual component rather than being two stages away as the DXF is.

If you increase the offset to 3mm it will most likely drop off everywhere then.

[martin54]

I know you are looking for an overall solution & this won't help with that but for this particular type of job could you not use the prism toolpath instead of creating & importing a model. For that style of lettering the whole job could be done in vcarve without any work rounds or other problems

[Lumenautica]

I know you are looking for an overall solution & this won't help with that but for this particular type of job could you not use the prism toolpath instead of creating & importing a model. For that style of lettering the whole job could be done in vcarve without any work rounds or other problems

with the Prism tool I've found it doesn't produce a uniform height along the spine so it reduces the height on the narrower sections of the letters which isn't desired for the application, so a model is required also we have to offer rendered designs for the customers to approve then this is used for manufacturing. previously I've had no issues with artcam I'm just trying to work out the best work flow for this type of work using V-Carve.

[Lumenautica]

Rather than using imported DXF's to create vector boundaries you may have better results using the Create Vector Boundary tool in VCarve. That way the boundary is created from the actual component rather than being two stages away as the DXF is.

If you increase the offset to 3mm it will most likely drop off everywhere then.

I need to relate the model profile to the dxf as we are making multi lamination signs.
I'm sure its just a setting I've not worked out. unfortunately I'm learning on the job as we go with this one.
I will set aside some time to refine the process and alignment issue.

[adze_cnc]

You may also find that the "offset" machining strategy may work out better than the raster one.