http://anthromod.com/blog/?p=98

Chris appears to have tried a number of rapid prototyping technologies and has started using the CNC/casting approach outlined at http://lcamtuf.coredump.cx/guerrilla_cnc1.shtml . That happens to be one of my favorite pages so I always look for reasons to link to it. You should check out both pages if you’re not familiar with the casting process.

http://www.kwartzlab.ca/2011/08/creating-3-dimensional-objects-taig-mill-rotary-axis/

He’s got a much cleaner work area than I do.

• 64 Bit Support
• A new “Automatic Toolpath Wizard” in the main toolpath dialog

We’ll use the part below to show how we can do a DXF to g code conversion with minimal effort:

This files contains a good combination of arcs, line segments and bezier curves.  Also, these is nesting where the rectangle and circle are within the outline curve.  MeshCAM will have no problem finding this hierarchy and generating a toolpath automatically.

Export the DXF

The first step in the DXF to g code process is the DXF file.  The DXF format has suffered a long evolution that makes it a less-than-ideal format to move CAD data between programs.  The “most compatible” version of this format was way back in Autocad Release 12, and that’s the one that MeshCAM likes to see.  Future MeshCAM releases will probably support newer DXF versions but V12 is the best one to use for wide compatibility with other programs.

Most CAD programs will have a list of DXF options available when you save the file.  In this example, we’re using the excellent Rhino CAD program but the lessons apply to almost any CAD program that can save 2D DXF files.

After saving clicking “Save As”, select a file type of “DXF”.  You’ll be shown this window:

Settings to use for a DXF from Rhino

Select the “R12 Lines & Arcs” option and you’re done.

Load the DXF in MeshCAM

Click “File” then “Open 2D DXF” and load the file saved above.  The file will be opened like any other 3D file with the exception of the new “Extrude” window:

The setting entered here will tell MeshCAM how thinck to make the new geometry.  If you’re just trying to cut flat stock then you should make the distance equal to the thickness of your stock.  For the example here, we’ll use .125″.

The new geometry created by extruding the DXF file .125" thick

It’s worth noting that this extrude command was added in MeshCAM V4.  V3 users will not have this command available.

Define Stock

The stock in MeshCAM is used to define the area in which the tool is allowed to move.  By default it is set to the size of the geometry you load (you can see it as the white box around the part).  In this case, the stock is touching the geometry so the tool would not be able to move completely around the part to cut it out.  We’ll enlarge the stock using the “CAM->Define Stock” command.

Since we just need to add a little room around the part, enter “.2″ for the “Right” and “Back” values under the “XY Position” area.  All other defaults are fine.

Only two settings need to be changed for the example here

In the screenshot below, you can see that the white box representing the stock has been enlarged.

The arrows show the areas where the tool now has room to move

Add Supports

The current settings would be fine if you’re going to hold the stock down with double-side tape or something similar.  What if you need to add tabs or other supports to hold the parts in place for machining?  Use the “CAM->Set Geometry Supports” command and enter the settings below:

Use these settings to define the supports

Click at a few spots around the part to automatically place supports.  Don’t worry if you get one or two of them wrong, you can right-click to remove the last support.  When you’re done it will look something like this:

Geometry with supports added

Generate a Toolpath

The only part left is the toolpath, and there’s not much to that.  Since we’re just looking to cut out a profile, we can skip the normal roughing and parallel finishing passes.  We’re going to use the waterline and pencil finishing only.  As a quick refresher on those two, waterline makes a series of profile passes around the part, each a little deeper than the last.  The only thing it does not do it attempt to find the “final depth” of the part to take a last cutout pass.  The pencil toolpath is used to trace the outline of the part one file time a full depth and ensure that nothing remains around the part.

We’ll use a .125″ endmill for both toolpaths and a stepdown of .03″ for the waterline pass.  The rest of the settings can be seen below:

Click to see a full-size version

Click “OK” and after a couple of seconds you’ll have a toolpath ready to go:

Completed toolpath

Way Faster than 2D

After you do this the first time, I think you’ll be agree that this is “way faster” than a traditional 2D CAM program that requires you to select vectors to cut or one that just does a straight DXF to g code conversion where no tool offsets are calculated.

Other Options

A couple of other options for advanced users:

1) If you want to plunge to full depth and cut the whole thing in one pass then skip the waterline and use only a pencil pass.

2) You can tell MeshCAM that the waterline tool is a little bigger than it really is.  This will cause it to offset the tool more than it should leave a little extra material around the part.  This lets the pencil pass cleanup the final surface in a single pass with a better finish.  For example, if you tell the waterline pass that your .125″ endmill is actually .135″, MeshCAM will leave .005″ for final cleanup.  This is one way that lying to MeshCAM can get you additional  features that were never programmed into it.  Don’t worry, it’ll forgive you.

All of that being said, it’s worth noting a few “quirks” about SW that make it slightly trickier to get a file out of than a program like Rhino.

File Types

MeshCAM Accepts 3D files as STL or DXF (using 3D Faces).  Of the two, STL is preferable since it is a more robust format and it is faster to read into MeshCAM.

STL is a file format originally developed for the 3D printer market that represents your models as a bunch of triangles.  Some users worry that some accuracy will be lost in the triangulation but this is not really the case.  As shown below, you can create the STL file to almost arbitrary accuracy- generally well beyond the accuracy of your mill.  Second, most CAM programs that take SolidWorks files natively do this triangulation in the background, it’s just hidden from you.

 Workplanes

The first thing that many users note when taking the output from SolidWorks to CAM software is the orientation of the parts.  As someone planning to machine a part after designing it, it’s tempting to build the part by extruding out from the “Top” plane.

Part built off of top plane

When you load the resulting STL file into MeshCAM you’ll see the following:

That same file loaded into MeshCAM

Obviously, this will require a rotation before machining it.  Within MeshCAM you can use the “Rotate Geometry” command to get the correct orientation.  You can enter an X rotation of “-90″ or, if you’re running MeshCAM Version 5, click the face button below:

MeshCAM Rotate Command

The simple option is to always extrude from the “Front” plane in SolidWorks.  If you do, you will always be able to load the STL directly into MeshCAM without rotation.

[EDIT] Randy just filled me on another technique that I never knew about- reference coordinate systems.  Under your Insert->Reference Geometry menu, select Coordinate System.  Place it in whatever location you want but align it so that the Z axis is parallel to the Z axis of your mill.  When you open the STL Options window, pick that new coordinate system using the pull down shown here:

The STL can use any reference coordinate system you've defined

Your STL will now have the proper orientation without any need to rotate it within MeshCAM.  Thanks Randy!

STL Units

Here’s a really frustrating thing in SolidWorks (if you don’t know about it)- the units of the STL are not necessarily the same as your part.

After you click “Save As” and select STL as the file type, click the “Options” button shown below.

When you get the options window open, note the “Unit” setting:

The unit value selected here will be used in your STL file no matter what units are used in your part file.  If  they differ, the part will be converted to the STL units when you save it.

STL Quality

The other major setting that affects the STL output is the “Resolution” setting defined in the “Export Options” window shown above.  The resolution values define how accurately the STL represents your original part file.

SolidWorks predefines a “coarse” and “fine” resolution and these will be fine for most users.  Unless you have a very large model I would usually recommend starting with the “Fine” option.

SolidWorks also gives you the option to define your own quality level using the “Angle” and “Deviation” sliders.  ”Angle” defines the maximum allowable angle between two triangles that originate from the same surface.  If that threshold is exceeded, smaller triangles are used.  The “Deviation” is the maximum allowable error allowable in the output.  Put another way, “deviation” is the maximum distance that a triangle can be from the surface that it represents.  For both settings, smaller values will give more accurate files at the expense of more triangles generate.  MeshCAM can handle very large STL files so you can definately use settings that are beyond the predefined “Fine” values and still have no problems.

Watertight/Solid STL files

Here is my one complaint about SolidWorks- it will not save surfaces as STL files, it will only save watertight solids.  To be fair, this is part of the STL standard and they follow that standard carefully.  If you have a surface model you will not be able to save it as an STL without finding a way to make it into a solid.

For what it’s worth, most other CAD programs will generate STL files from surfaces and MeshCAM will happily machine them.

Conclusion

Hopefully this is enough to get new users over a few of the difficult starting points to get going with SolidWorks CAM.  Be sure to post in the comments in there is anything else that should be added.

While there is a certain “elegance” if you’re an engineer, it’s a wall of grey numbers to normal people.  Below is the new version which retains almost all of the functionality with far fewer buttons and numbers:

I think it’s better but I guess I’ll know for sure once new users begin playing with it.  I didn’t delete the old code just in case…

What is an Undercut

An undercut is an area of a model where one part overhangs another part, creating a void in the middle that cannot be reached by a traditional 3-axis mill or router.  That probably sounds like gibberish so here’s a picture-

That “hook” creates an area between it and the back plate that cannot be machined.  You’d have to leave a section unmachined or break it into multiple parts and bolt or glue it together.

It’s worth noting that an “undercut” is specific to a direction of machining.  The part above only has an undercut if you machine it from the top or the back.  You could flip it on it’s side to machine it but that’s not really a cure all- I could easily come up with a part where that is not possible.  We’re using a simple part here to illustrate a point.

Special Tools

Special tools are sometimes used to machine simple undercuts. These are sometimes called “slot cutters” or “lollipop cutters” depending on their shape. Both tools feature a tip that is wider than the shaft. This gives the machinist some limited ability to reach into the undercut- but only by the difference between the tip and shaft diameter. For many uses this will be fine but it is certainly not a universal solution.

A big negative for these tools is that most CAM software does not support them directly. Because these special cutters are infrequently used, only the hig-end CAM programs include algorithms that can utilize them. For the rest of us, special cutters require manual gcode, tricking the CAM program, or moving the mill manually.  I’ve never had a case where their use outweighed their negatives.

One Example of a lollipop cutter

It’s easy to see that the cutter above may not have the reach to machine the whole undercut in our example part.  Surely there’s another way…

Think Like a Plastics Engineer

I spent years as an electrical engineer working with factories in China, ignoring the plastic and mechanical parts of my projects.  One day a friend of mine showed me how he modified a part to eliminate a small undercut that would cause excessive wear in one of our molds. It was a common practice for plastic injection molding but it was not something that ever occurred to me- cut a hole in the back of the part for a tool to get in.  In retrospect it was obvious but it wasn’t something I ever spent much time thinking about.

This access hole in the back of the part allows you to flip the part over and machine the undercut from the back.   MeshCAM has a built-in “two-side job” type that makes this really easy.  Below is what the front and back toolpaths might look like:

Toolpath when cutting the top of the part

Toolpath when cut from the bottom of the part.

The red arrow shows where the tool is now able to access the undercut and remove that material.

A More Complicated Part

The same technique above can be applied to more complicated parts that would be much more difficult to machine in their “standard” configuration.  Here’s one one of those, half a hinge:

Half of a hinge with no undercuts

The hinge is now easy to machine from two sides and would be easy to mold if necessary without slides or inserts.  It’s not exactly going to work for a restoration job on an antique piece of furniture but it’s still a cool trick.

Play with Toys

If you have kids then you’re probably going through toys at a rapid pace, try opening a few up and looking at how they are designed.  You will likely be shocked at the number of shortcut and tricks used to make complicated mechanisms that can be produced in simple injection molds without undercuts.  Most of these injection molding tricks are applicable to the milling process as well.

Not a Cure for Every Case

Cutting a hole in a part is not going to work every time but it does work more often than you think and it’s one of the easiest ways to machine a difficult part.

That’s a peak usage of 5 GB of memory without a crash.  The model used in that test was a 12 foot diameter sphere machined with a 2mm stepover at a .001” tolerance.

When packed into the existing installer the 64 bit build only adds about 3MB to the file size.  That’s pretty insignificant so I’m going to stay with a single installer for both 32 and 64 bit builds.  64 bit users will be able to pick which version to use while 32 bit users will automatically be given that version.

To get this build working I had to make hundreds of little changes so this build officially marks the start of MeshCAM V5 development.  It won’t be done anytime soon but I will try to get some betas flowing over the next couple of months. 

The following post focuses mostly on 3D toolpaths so we’ll be assuming the use of a ball mill.  Once you understand the basic concepts it’s easy to apply them to flat end mills and bull mills.  We’ll try to build to some rules of thumb rather than derive equations that most users won’t be interested in.

Definition of Stepover

Almost all CNC toolpaths are based on the concept of one toolpath being offset from another by some distance; this offset distance is generally called the stepover. Most CAM software, MeshCAM included, uses a couple toolpath styles in particular with these offsets- the raster toolpath (sometimes called a zig-zag toolpath) and a contour offset.

A contour offset toolpath

A raster or zig-zag toolpath

Adjacent sections of the toolpaths above are separated by the stepover value chosen by the user.

Scalloping

The pictures above show how a toolpath is arranged from above but a side view clearly shows the primary side effect of your stepover choice- scalloping.

Scallop shown in red between adjacent passes

The area in red is the part of the stock leftover on the part in between the toolpath offsets.  It’s important to understand that these are not good; they are not in the CAD and may need to be removed after machining by sanding or polishing.  CNC machinists are almost always trying to reduce the scalloping as much as possible and many man-years of effort have been spent trying to develop toolpath algorithms that minimize them.

Scallop vs. Stepover

A moment spent looking at the image above illustrates at connection between scallop height and the stepover value- increase one and the other increases as well.  In the images below we’ll use a stepover equal to 1/10, 1/5, and 1/3 of the tool diameter to show this correlation.  To put real numbers on this, that would be equavalent to a .012,  .025, and .042″ stepover for a .125″ ball mill.

Stepover =1/10 of diameter

Stepover =1/5 of diameter

Stepover =1/3 of diameter

As you can see, the change in quality is so dramatic that you might be tempted to always use the smallest stepover possible.

Speed vs Quality

It shouldn’t be surprising that you’ll have to give something up if you want to use a really small stepover.  In this case you’ll trade time for quality- you give up machining speed to use a small stepover or give up quality if you want a quick machining time.  This is easy to understand when you consider that the total length of a toolpath will approximately double if you cut the stepover in half.  The question is, “Will cutting the stepover in half double the quality of my part?”

The Sweet Spot

It turns out that there is a point of diminishing returns in the time/quality tradeoff.  Below is a graph of scallop height vs stepover that illustrates the effect.  The graph has been normalized to a tool diameter of 1.0 so it’s easy to scale it to any tool you happen to be using. (Click on it to see a bigger version)

Scallop vs. tool diameter

The important thing to note is the shape of the graph- it tends to flatten out when the stepover goes below about one eighth of the diameter.  This means that when you go below this point you’re going to take more time to machine without a proportional gain in finish quality.  If you’re machining a steel injection mold then it may still be worth it but you really need to be sure before doing that.

Scallop vs. Tool Diameter

Here’s the other thing we can glean from the math behind the chart above- for a given stepover, a larger tool will give you a smaller scallop.  This means that you can get a better finish “for free” if you can use a larger tool.  Obviously, this only works if a bigger tool will fit into all of the parts of your geometry but this is one of the few “win-win” things we can do get better results if it does work for your geometry.

Scallop with a small tool

Note the reduced scallop when a bigger tool is used even though the stepover is constant.

Keep the Material in Mind

Before you figure out what stepover you need to get a .0001″ scallop, think about what you are going to machine- wood, tooling board, aluminum, steel, etc.  I can tell you that in many cases you can do 10 minutes of sanding on a wood part to get a finish that would have taken you an extra hour or two to get straight from the mill.  Likewise, tooling board like Renshape can be hand finished quickly enough that it may not be worth doubling the machining time to get a better finish.  If you’re cutting steel or other hard materials then it’s probably worth letting the mill do more of the hard work.

The second characteristic of the material to consider is what kind of detail it can hold.  MDF will not hold features in the .01″ range but metal will. If your material cannot hold a detail that is smaller than your scallop height then you do not need to reduce the stepover; doing so will only waste your time without producing a better finish.

Keep the CNC Machine in Mind

It may be a poor craftsman that blames his tools but we do have to be realistic about the nature of our equipment.  In particular, how long do you trust your mill or router to run trouble-free?  I started out with a small table-top mill that, while very good, could not be trusted to run for hours without missing a step or hiccuping in some way that gouged a part I had waited half a day to get.  If you have a machine like this then it’s worth thinking about the picking the maximum stepover based more on machining time than finish.

Rules of Thumb

That was a nice bunch of pictures but you may still be left with the question, “So what stepover do I use?”  Here are a few suggestions:

• The stepover should be between 1/3 and 1/10 of the tool diameter
• Use a larger stepover, in the 1/5 to 1/3 range, for soft materials that cannot hold detail well
• Use a smaller stepover, in the 1/5 to 1/10 range, for hard materials or materials that can hold significant detail like metal and jewelers wax
• Use the largest tool that will allow you to machine your geometry

Once you have a few projects complete you can adjust the guidelines above to suit you materials and machine.

Here it is CNC Milling Feeds and Speeds Cookbook