The Hell Ya Beller Fun with hot, pointy, sharp, and caustic stuff.


Understanding My Enemy

My interests in CNC and machining developed over a period of years in a very organic way.  I have no formal training in either engineering or manufacturing --my interests were born out of necessity.   Learning that way is great if you have the time and patience.  Sometimes, however,  it's just frustrating.  You find yourself struggling with something that should be easy and only later find out that all kinds of people have the same issue and either they know how to work around it or perhaps they just feel each other's pain.  But you, the loner, are left banging your head against the wall feeling like an idiot.

Meet the Spider

This post is about a perennial problem that I've faced in lots of CNC projects.  It's something newbies like me are going to see eventually so this post is for you.  I don't know if this problem  has a name so I call it the 'spider problem'.  If you know anything about this or how other CAM packages address it, leave a comment.

The first time I saw it was when I was playing with the HeeksCNC zigzag operation. To mill the spider, a lot of material needs to be removed but there are some areas that are very small and require a small cutter to reach.  And there lies the problem.  If you use a big cutter to go fast, you can't get into all the nooks and crannies like the space between the legs.  You end up with a tool path that looks like this:

Figure 1: Detail, especially between the legs is lost.

If you choose a small cutter that can get in there, your step over and step-down values have to be small.  The run-time on the job is going to be excessively long - really REALLY long.

Figure 2 - A small cutter needs small step-over and step-down. The resulting path is huge and the run time will be very long.

Roughing and Finishing

The intuitive solution is to rough the spider out with the big cutter, then do a finishing pass with the small cutter.  With a model that doesn't have all those tight corners, this works great.  It's exactly the technique I used on this pinewood derby car.

But it doesn't work here. Finishing assumes that the roughing phase has left a small, roughly uniform amount of material all over the model.  The finish pass doesn't limit step-down because it doesn't have to.  Ideally you're already within one step-down distance of the model everywhere.  Cutting our spider, we're within one-step-down everywhere except the small areas between the legs.  There, the remaining material is 5, 10, or more step increments away -- we're still roughing in those areas.

Figure 3 - A finishing toolpath has the detail we need but it's deceptive. Areas between the legs look like finishing paths but are actually roughing.

Of course you can limit the step down value but now you're back to where you started.  You're either spending a LOT of time milling air, or you're plunging your cutter and breaking it off.

The fundamental problem is that the CAM software doesn't know what material has been removed.


Manually controlling the boundaries.

The only other solution I've found, and one I use regularly, is to artificially limit the boundaries of the operation.  This means creating some geometry -- a sketch -- to limit the work area of of a roughing operation.  For instance, I could create a boundary sketch like this:

Figure 4 - A manually drawn bounding box can be used to limit cutter movement to the areas that need additional roughing.

The resulting toolpath will focus on the problem areas.  This works but it's a compromise.  If the model is complicated with lots of small problem areas, it can be difficult or impossible to create the right kinds of boundaries.  It's also manually intensive and, at least in my case, that means mistakes are likely.

Not just about 3D sculpting.

The example I've given might make it seem like this problem is only about milling 3D irregular models but it isn't.  Imagine cutting a simple rectangular pocket.  If the pocket is large, you'll want to use a big cutter to remove a lot of material but you'll have rounded corners with the radius of the cutter.  If you use a small cutter to get in tighter, you'll either spend a lot of time milling or you'll have to add some artificial bounding geometry to keep your itty-bitty cutter working in the corner and not milling air that the big cutter already cleared.  The problem is the same and the available solutions are the same too.  All compromises.

What would a better solution look like?

A smarter CAM tool would remember where previous operations had sent the tool and avoid re-milling those areas in subsequent operations.  The workflow I would like to see would look like this:

1) The user selects the model and creates a roughing operation,  specifying the tool to use and the feeds and speeds. The boundaries of the model are used to determine the work envelope.  The step-over and step-down could be suggested from the tool or overriden by the user.

2) The user selects the previous operation and creates a refinement operation.  The user selects the tool, feeds,speeds, and step-overs just like above.

3) Optionally, additional refinements can be added with progressively smaller tools, each time, the refinement references the previous operation not the original model.

4) When the tool path is generated, the system first generates the roughing operation tool path.  It then constructs a solid in memory using the bounds of the path - the area swept out be the tool.  It performs a boolean operation comparing the new solid to the original model to see where material still remains to be cleared.  The resulting area, or its perimeter at least, is used as the bounding box for the refinement operation.

5). The user selects the original model and adds a finishing operation, which works just like it does today.

I'm sure there's a lot I'm missing in this approach -- maybe even some legitimate reasons it won't work at all -- but I'm listening and willing to learn.


Comments (3) Trackbacks (0)
  1. Posted a while back but I just saw this and there were no comments, so here goes. The feature you are looking for is called “Rest Mill.” In cam software that keeps track of stock removal it is “fairly easy” to use several tools in successive operations and tell the cam system to ‘get the rest of it’, hence “Rest Mill.” This is not the simplest thing to do if you are not a computer that can run through hundreds of algorithm iterations quickly. What it comes down to, however, is pretty much just a refined version of what you’ve laid out.

    Perhaps you could “blob” a model (enlarge and round out) to something that could be cut effectively with a larger tool and then use the “blob” as a 3D stock boundary around the final model…

  2. Thanks. I haven’t heard that term used but I’ll Google it for more examples and for details on how it’s done. HeeksCNC doesn’t have the concept of a stock boundary but I agree something like that is needed to accomplish this.

  3. Also some CAM use a Dynamic Stock Model which not only knows how the stock looks at the start and end of each toolpath, but also keeps track of this all the way during the toolpath calculations. Very efficient for machining time as well as safe and less change of gouging

Leave a comment

No trackbacks yet.