What is Machining Margin in MeshCAM?

Hi, well the title says it all really. What value should be set for the machining margin? Or more importantly,what does it mean?

The machining margin is how far outside the geometry outline MeshCAM will take the cutter axis. I usually set margin at about 3/4 the cutter diameter. 3/4 of the cutter diameter leaves a reasonable kerf for clearing chips. Anything more just makes a larger kerf around the part. When you’re using perimeter supports you also want to minimize the kerf to avoid sudden lateral moves into the raw stock when the cutter gets down to the level of the support. That has been brought up in another thread.

On 3D parts with a variable-depth “equator” line, I like to use a margin of just less than the cutter radius. With a ball-end mill, this will machine almost to the edge of the part, and the cutter will not “fall off the edge”. There will be a little cusp to hand-finish but this can avoid a lot of extra machining time becuase the cutter only goes as deep as necessary at each point of the perimeter, rather than a maximum depth that might be excessive for some areas of the part.


1 Like

Thanks Randy, that clears it up well. So if my stock only slightly larger than the job (less than a cutter width say) I could set it to zero?

I’m going spare watching my cutter machining air all around my part… grr.

So if my stock only slightly larger than the job (less than a cutter width say) I could set it to zero?

If you aren’t machining the perimeter of your part, you can set the margin to zero. The cutter axis will stop at the boundary of your part and only machine the top and any internal cavities.

If you want to machine the perimeter of the part, you need to specify a margin of at least your cutter radius. If the perimeter of your part is a vertical wall, and will be machined entirely by waterline and pencil finishing (no roughing or parallel finishing) you can make the margin as large as you wish, becuase the waterline and pencil finishing will follow the shape of your part anyway.


Thanks Randy, as usual that is a very helpful answer. I would very much like to see some of the work you do. You seem to be extremely competent on this machine.


If I have a piece of wood that I want to leave the size it is, and just cut a pattern on the surface, would I set machining margin to zero?

If I want to cut out a 2D part from a flat piece of stock would I set machine margin to half the cutter diameter?

When I am cutting a pattern into stock that I do not want to trim the outside edges of my machining margin is a standard diameter of the cutter and then the cutter spends a lot of time running around the outside of the stock cutting nothing.

I think I understand what you said above, but want to check with a couple of examples to be sure.



@1st_Kiwi_Nomad, I’m not really experienced on the Nomad yet, but I’ve been using MeshCAM since the early betas. I’ve machined parts on a Sherline mill, an Isel gantry table, a Tormach mill and now the Nomad. I have sleep apnia, and every night I use a custom nose mask I’ve designed and machined in 3D with MeshCAM (I’m on my 11th prototype). The most extensive machining I’ve done on the Nomad is on my model railroad bridge mockup, which I’ve machined from stock styrene shapes. This is where it stands now

and from here on I’ll add bracing members hand-cut from thin strips of styrene. But the Nomad machining involved cutting pockets in the wasteboard, indexed machining of the main beams which are longer than the X travel, etc. It has been a good learning experience.

The biggest 3D machining was my ill-fated Millenium Falcon, which led to discovering the step generation errors, but I haven’t gone back and done a successful machinng yet.


  1. For the surface pattern, yes, specify Machine Whole Stock with a margin of zero. The cutter will not machine around the perimeter of your stock.

  2. For a 2D part (i.e. only waterline and pencil finishing) you can specify any margin you wish as long as it is larger than your cutter radius. Waterline and pencil finishing will “hug” the vertical walls of your part and not stray outwards. Now if you are using geometry supports, you will want to use a margin just slightly greater than your cutter radius, becuase MC will follow the supports out to the margin.

It is instructive to play with these variables and look at the toolpaths that MeshCAM shows at the completion of its calculations. You don’t need to see the simulation to discover whether or not MC is generating toolpaths at the perimeter of your stock. I do trial runs and look at the toolpaths all the time when I’m helping people with toolpath questions. I’m not actually omniscient :wink: but it is pretty straightforward to experiment with settings. :smile: I encourage it for everyone. On a new workpiece, I’ll ususally go through 4 or 6 iterations before I get toolpaths I’m happy with.


Wow that’s really interesting Randy, I have a good friend that works for Fisher and Paykel Healthcare here in New Zealand where they make some of the best OSA machines in the world. I know that the mask development team is just non stop creating new mask designs. They have hass mills nocking out aluminium injections molding tools for 1000 off prototype runs one after another. It would be fun doing that sort of volume tool making I reckon. Did you actually machine your protoype masks or molds to mold them from silicone or similar in? Sucks that you have sleep Apnia though by the way but what a crazy practical way to use your CNC skills!! I can’t sleep because I spend too long trawling this forum, and what’s amazing is I can remember only a few months back when it was new and I’d read every post - not any longer though, not by a long shot!

well actually it’s been a year… just saw I have had my anniversary badge for one day :smile:

1 Like