First 3D carve

[Schreib]

Hey everyone, I'm about to do my first 3D carve, I typically 2D everything but wanted to try and 3D carve something that was simple for my first round except the model preview is showing a lip left over after doing the carve and not not sure how to get rid of it, thought it was my boundary being to close to the profile at first but that doesn't seem to of been the cause.

Ive attached a photo and the file for review.

[sharkcutup]

You do either of two things ----

1.) Offset Outside Profile Vector Inwards a bit then recalculate Profile Toolpath

OR

2.) Select Inside/Left and Re-Calculate Profile Toolpath

Sharkcutup

[Schreib]

doing that makes the overall dimensions smaller than intended, there should be another way.

[sharkcutup]

You could make your material board an little larger to allow for the Outside Profile cut thereby maintaining your required Dimensions!!! this would give material also for your hold down clamps of course that is if you are not using a Vacuum table.

Sharkcutup

[adze_cnc]

The centre of the finishing bit in a 3D finishing tool-path stops at the model boundary or selected vector (depending which you’ve used) leaving that flared edge.

To get rid of the flare you need to convince the software to cut past the centre of the bit to partially “roll over” the edge. The setting for that is the “Boundary offset”. Try a titch smaller than the bit radius and decrease it if the bit goes over the edge and tries to cut the small vertical face that it appears that you might have. (I haven’t had a chance to look at your file.)

[adze_cnc]

Now that I've had a chance to look at your original file I notice that not only do you have a huge "Boundary offset" (1/2" bit diameter) but that you've even offset the "Selected Vectors" a 1/2" beyond the the 3D model meaning the centre of the bit should extend 1" beyond the edge of the model.

You were getting the flare no matter what you did because your model and material size are the same. The finishing toolpath is not calculating beyond the material boundary. So, Sharkcutup's suggestion of increasing the material size is the way to go. He just didn't provide enough background for you to apply it.

I only have a trial version of the 11.5 software so I can't upload the file here. But, we can see in the images the steps I took.

What we will do is lie to the software and tell it that the material is larger than it really is. But we will adjust things so that origin point (0,0) is at the corner of your actual material (marked by the blue arrow).
 

 
I've made the width and height 1 inch larger than your actual material. Note the -0.5, -0.5 offset is to move the fake material away from the actual corner of your material (pointed to be the blue arrow).

After changing the job dimensions and origin-offset your vectors and 3D model will be in the wrong place. Turn on all the layers, highlight all the objects and press "F9" to centre them in the new "false" material envelope.
 

 
Note that I have moved you highly offset vectors into the "_not needed" layer (coloured in red). I've moved the vector that is the outside boundary of your 3D model and the vector in the "Hide" layer to the "3D boundary" layer.

The "Rough Machining" toolpath settings are here:
 

 
The biggest changes are:

• Boundary offset can be set to zero (0)
• I changed the Raster angle to 90 to maximize the amount of time it will cut long strokes and minimize the time it cuts small zig-zags
• Use the Vector Selection "Selector" button to choose items on the 3D boundary layer instead manually selecting them

The Finish Machining Toolpath settings are shown in the two images below:
 

 
The tool's stepover has been set to 0.045 from your 0.050 and the Boundary offset set to 0.225. The 0.225 is to allow the tool to roll over the edge as I mentioned in my previous post. The 0.045 is found from taking the distance between the boundary vectors (1.125) and dividing by 25. If we take the 1.125 and divide by 0.050 we get 22.5 passes. Because of the 1/2 pass there might be an unsightly artefact line. But by changing the setting to 0.045 we get a whole number of passes. I could have divided 1.125 by 23 to get 0.048913 but that seemed annoying.

The vector selection is the same as the roughing:
 

 
This is a simulation of all the cuts (I kept your profile cut the same):
 

 
I hope this helps.

Steven

[sharkcutup]

So, Sharkcutup's suggestion of increasing the material size is the way to go. He just didn't provide enough background for you to apply it.

Thank You Steven For your help/Input, I was in a bit of a hurry earlier!

Sharkcutup

[Schreib]

So, Sharkcutup's suggestion of increasing the material size is the way to go. He just didn't provide enough background for you to apply it.

Thank You Steven For your help/Input, I was in a bit of a hurry earlier!

Sharkcutup

Appreciate your input earlier i did end up getting it but I figured it out on my own i suppose but reading back this makes since.

[Schreib]

The centre of the finishing bit in a 3D finishing tool-path stops at the model boundary or selected vector (depending which you’ve used) leaving that flared edge.

To get rid of the flare you need to convince the software to cut past the centre of the bit to partially “roll over” the edge. The setting for that is the “Boundary offset”. Try a titch smaller than the bit radius and decrease it if the bit goes over the edge and tries to cut the small vertical face that it appears that you might have. (I haven’t had a chance to look at your file.)

Appreciate it, I did end up doing more troubleshooting after my first reply and went to increased the material size and then doing a xy offset to set it back to zero so I could still put the material in my normal zero position, and it all worked out, though one thing did happen when I made this cut is that the finishing tool pathing came up to the top and cut about a 0.5in by maybe 5thousanths off the top around the lip not sure why since I had a boundary set up on the edge. Was able to sand it down but I didn't want it to do that at all.
Any ideas?