Adjusting for Kerf in your Design Parametrically - Fusion 360

I was going to link to another topic that has (once again) disappeared, so be sure to check out the tutorials on kerf from @smcgathyfay and @Hirudin for a discussion of what kerf is, and how it impacts design.

If you’re just getting into Fusion 360, a good way to pick it up quickly is to watch a few of the Fusion 360 Training tutorials on YouTube:


Okay adjusting your sketches for kerf is fairly easy. If I had something like a hole that had to hit an exact diameter after cutting, I would probably do something like this:

Open the dimensioned sketch.
This shows the exact size that you want things to be when you’re done. 50 mm hole.


Modify > Change Parameters


Create two new User Parameters by clicking on the green plus sign to add them:

  1. kerf
    Expression = 0.20 mm

  2. half
    Expression = kerf/2

(You can also just name these “k” and “h” to speed up the typing once you’ve done a few.)

Click OK to save the values.


Select the dimension for the circle.

(The index lines are added here for display purposes only, to show the original size desired.)

If you want the hole that is being cut to remain the same size, change the formula to read:
dimension - kerf

If you are cutting out around the post in the center of the hole, change the formula to read:
dimension + kerf

If you now export the DXF of the sketch for use in the Glowforge, you will have adjusted your holes for a kerf of 0.20 mm. You can use that DXF on any non-Proofgrade material.


If you find out later that the kerf on that material is actually 0.25 mm instead of 0.20 mm, you can now go into:

  1. Modify>Change Parameters and change the kerf Expression value to 0.25 mm.

  2. Everything instantly adjusts automatically :smiley: – export the DXF.


So you can actually see what is going on here – let’s bump the kerf to 3 mm:

(And I’ve added a little centered red laser dot equal to the kerf to show the edges of the path. Again, just for display.)

Kerf = 3mm

And when you’re done, or want to use Proofgrade material:

Kerf = 0

Back to where you started. Nothing destroyed. Nothing changed.

Alternate Method:

Choosing to cut outside of a shape like a CAM toolpath does.

Making this parametric requires an additional step or two, since the Offset is actually a new line creation, not a modification of an existing path.

(And you’d better believe it took me a while to figure that one out yesterday.):unamused:

The steps are:

  1. Double click on one of the lines in the closed shape to select all of the paths in it at once

  2. Sketch > Offset

  3. Drag the slider in the direction that you want to shift the path (Outside if you are cutting around a shape, and you want to maintain the exact dimensions of that shape. Inside if you wish to maintain the exact dimensions of a hole in your shape.)

  4. Don’t worry about the value of the Offset position yet – you are just creating a template.

  5. Click OK


  1. Hover the mouse over the dimension for the relationship that you just created. Make note of the name of that dimension : d35

  1. Go back to Modify> Change Parameters and drop down the Model Parameters list.

  2. Change the Expression value to half for d35. (And any other offsets you have created.)

(You’ll see the value change to reflect the parameter value up top in the User Parameters section.)

  1. Click OK.

That’s it! You can now drop in one kerf number, whatever it is, and your file is going to adjust itself to cut correctly, without you having to tell another program that you want this line to cut on the inside and that one to cut on the outside!

Export the DXF, and you’re ready to convert it for the laser.

Some examples just for show:

For kerf = 0.20 mm (actual laser kerf)


For kerf = 8.0 mm (big enough to see)


And when you’re done exporting your results for conversion, to go back to your single lines, the ever popular kerf = 0, and your file is back the way it was when you started.


Tips to speed it up:

When you are setting up your Offset templates for these things, this particular program requires you to do them one at a time, but you can speed up the process nicely by doing them all in one big batch, so that the names of the offset functions are numbered sequentially. Then just find one and you can change all of the Expressions to half at the same time.
(It saves a lot of flipping back and forth.)

Right mouse click, hold, and drag straight up to repeat a function. That’s just the way Fusion 360 works, but if you’re setting a lot of Offset templates on a bunch of different parts on a page, it saves a lot of clicking.

Okay a couple of comments, which I claim the right to, by virtue of having taken the time to put this together.

If you’ve read all the way through to this point, you’re interested in how kerf-adjustments are going to work, but since this is a tutorial, let’s please not clutter up the comments section with arguments for or against Glowforge doing something similar with their interface. Go argue whether they should have one or not in the other thread, where your vote can be counted.

For newcomers to 3D design:
Without going into a scary amount of detail - I’m going to point out that this kerf “fix” only addresses 2 of the 3 dimensions that you have to take into account in your designing. The third dimension, thickness, also has to be accounted for in your designs, and this method does not address it.

You do not want to see what that involves. :wink:

And last: If I’ve misunderstood what you guys are trying to accomplish…sorry about that. This was new to me yesterday.

Feel free to clarify. :slight_smile:


Better yet, start a new thread to discuss the CAM vs Manual etc.


Awesome post! May have to revisit Fusion 360…:smirk:


Big kudos to you for all the work of putting this together!

Thank you so much, I look forward to diving into this further when I get home.


It’s a booger to get comfortable with, and then…bam! Instant whiz-bang!

The video tutorials really help!


That isn’t the optimum tool path for kerf adjustment. The corners should be rounded with a radius equal to the half the kerf. That is the path that is a constant half kerf offset from the perimeter and is smoother motion for a machine to follow.


Absolutely true. And for a kerf of 0.2 mm, I am going to completely ignore the radius on it. :slightly_smiling_face:

Also a laser is not going to bind at all - it is a beam of light.


huh? Can you draw something up real quick to illustrate your point? Are you talking about dogbones (I think that’s what they are called, little circles in the corners to help the piece not crack under pressure), or are you talking about just simply eliminating 90 degree corners with small curves to prevent the laser from stopping and pumping more laser into the inner corners of the object?

1 Like

I’m talking about the slight curve that is left behind in a 90° corner because a rounded tool can’t go into it. (Too small to bother with.)


This is true…the laser can do sharp 90° angles unlike a round bit.


Wonderful tutorial…very detailed and easy to follow!! Thanks so much for taking the time to put it together. Guess who’s just found a new way to procrastinate grad school prep by watching Fusion 360 tutorials…


No it can’t. It’s a round spot so it leaves a corner radius just the same as rounded tool. It is just very small, that’s all.


The path should look like this (spot radius exaggerated).

The outer line is the tool path. The inner line is the shape it will cut. Note that internal corners will have a radius equal to the spot.


That was a good example, especially showing the square outside corners. That can be a confusing concept to grasp.


Okay, first, you are awesome. You may not be the very most knowledgeable person here but your willingness to actively share what you do know is inspiring.

So, two things. First, I got from some of @smcgathyfay sharing that won’t box joints need two separate adjustments?
Second, well you have gone this far, you might as well go whole hog and explain in three dimentions.

Thanx again!!


Coincidentally, dog-bones got mentioned earlier…I believe that Fusion 360 has an automatic dog-bones app that you can run to include them on all applicable corners after you finish your design.

I haven’t used it, (or found it for that matter), but I saw it demonstrated in one of those videos.

I need to go see if I can find that.


Oh, yeah, I should have mentioned that…if you apply the Offset to one part that you are cutting, you need to apply an Offset to all of the other pieces of the box as well. All the half offset does is move the laser beam out just far enough that the edge of the beam contacts the line that you originally wanted to be your outside edge, instead of the center of the beam.

The reason why you would get a full kerf of difference between two joining parts without adjusting for kerf, is that exactly half of the kerf gets removed from each piece when it cuts.

But you do have to apply it across the board, or you are still gonna be missing half on one part.

Good catch!

Not even for a free Glowforge! ROFL! :smile:


The laser beam is a merely a hair’s width… big difference than when using a router bit. You can zoom in on the cuts that I make with my lasers and unless you are making microscopic designs, the “roundness” of the laser beam is virtually non-existent.

Curious, what laser are you running that you get rounded corners on the outside of your cuts?

I can see how this would be important to know when using a bit to cut with…but in all honesty it seems like splitting hairs in this case.

1 Like

I don’t have a laser because my Glowforge hasn’t arrived yet :disappointed:

This is a close up of a laser cut slot in 2mm acrylic. It’s 2mm deep.

This is a human hair at the same scale.


Nice that you brought that up, because I think THAT is what the Glowforge is going to do for us - the focusing part.

They will auto-focus the laser for us so that the kerf is minimized to the size of that hair, straight up and down. (to the extent that it can, depending on the thickness of the material and variations in manufacturing, yadda-yadda-yadda)

We should get a much better cut than what shows in that image, I would think.

That is the “little black book” part of the equation.

Feel free to jump in here and correct me if I have that wrong…because that is what I’m holding out for…

Focal distance.

(That would be another pile of stuff to have to learn.)