Allikas: Digilabor



To mill out your parts from plastic blank sheet, we need to generate G-code for mill. This can be achieved with fusion's CAM feature. This document describes most important properties and methods how to prepare your designs for milling.


To start creating a CAM job for your design, you should select CAM from left upper menu:


Now you should see new toolbar with different CAM related tools:


Job setup

First thing to do is to create a new setup for your job. For this, choose setup -> new setup from toolbar:


You should now set stock properties and origin point (the point where the milling job starts). Stock should not have any padding and the starting point should be from left top corner of your part. Z axis should point up, X and Y axis should point along the sides of your part. Final result should be something like shown on these images: Here you can see a version, where part's orientation is already correct one:


On this image the correct orientation is chosen by selecting reference face for Z and edge for X axis. Additionaly, "Flip X Axis" option was required. In your case, it can be different options.


Another important thing here is to set stock offets to 0 from Stock tab from setup options panel:


Now you can click OK, and you have created your first setup for milling job.


Different milling operations can be made from toolbar (most used in our case are tools from 2D and Drilling).

First we want to drill all the holes that are on your part. This can be done by choosing DRILLING from toolbar. Now, from DRILL panel, first thing to do is to choose a tool as follows. This one is for drilling 3mm holes:


NB! Refer to the exact tool with correct properties (cutting feedrate, plunge feedrate, surface speed etc).

Now select next tab from DRILL panel and you can select the holes which you want to be drilled. You should select hole face.


Now select last tab from DRILL panel (Cycle) and select options like following:



2D contours

Next operations should be inner slots and cutouts from your part. For this, let's choose 2D -> 2D contour from the toolbar.

Tool selection. If your part's inner contours (holes) contain only contours that can be milled with 3mm flat end mill, then you can choose same tool as before in the drilling section. Otherwise, if you have smaller contours then lets choose smaller tool. Here, in digilab, we have 1/16inch endmill:


From next tab, lets choose properties like shown on this image:


The "Tabs" option is not required for small inner cutouts. Main purpose for this option is that big objects that are cut out will not "fly" away while mill is still running.

Now you can choose the contours you'd like to cut out by selecting bottom edge of a contour like this:



It's very important to inspect the arrow - it should be pointing along the edge inside the hole.

Next thing to do, is to open fourth tab from 2D CONTOUR panel (Passes) and tick "Multiple Depths" option from there. Check tool settings table for "Maximum roughing stepdown".


Uncheck Lead-In and Lead-Out from fifth tab (Linking).


If you have done your inner contours, for the final step you should do outer contours following the same instructions. It is very important that the last operation that mill is doing is cutting out outer edges!

Checking the results

Now that you have created your CAM job, you can quicky ckeck it for any obvious mistakes. Simulating helps with that. Not only does it tell you, how long the job will take, but allows you to see how exactly it will start to cut the material.


1) The simulate button can be found there.

2) To simulate the whole CAM project, select your root setup, otherwise you can select one of the subjobs. For this example I selected the root setup.

3) Here you can control the speed of playback and see the time distribution of different jobs in the shape of the line in the bottom of the screen.

4) Here is the simulation control panel. Turn on "Stock" to see the raw material.


Once Stock is turned on, what you will see is similar to this picture. If any cut is unexpected, you can see it here too. The yellow and red lines are movement and blue lines are the cutting path.

Post process

Now that you have done with all operations with your part you can post process by right-clicking on setup from left tree-structure and choosing "Post process". From there (if you are doing this for the first time) you should browse for post processor (download link here) folder. After that you should be able to choose easel post processor from select drop-down menu.

Now click "Post" and you should have correct file for importing in easel. Easel is browser tool in which you can import the g-code and run x-carve mill. All the necessary software is installed on the desktop computer next to mill in digilab.

Tool settings

Material: Polycarbonate

Plastics work better with higher feedrates, at low feedrates the material might start to melt from excessive heat generated by the tool spending too much time in one place.

Following settings are good starting points that have been used before.

Tool Operation Cutting Feedrate Plunge Feedrate Maximum Stepdown
3 mm flat endmill Drilling 200 mm/min
3 mm flat endmill Milling 1000 mm/min 100 mm/min 1 mm
1/16" (~1.6 mm) flat endmill Milling 200 mm/min 50 mm/min 1 mm


Tool size

Largest available diameter tool size should be used based on smallest inner radius. Larger diameter tools are more rigid and can remove more material in the same time.

Tool count

Using least amount of different tools allows to save time by avoiding tool changes. One option is to design inner radiuses to be as large as possible to avoid using smaller diameter tools.

Tool changes

If different tools have to be used then it is recommended to order the operations by grouping together those that use the same tool.


Not good:

  1. Drilling with 3mm endmill.
  2. Toolchange
  3. Milling inner contours with 1/16" endmill.
  4. Toolchange
  5. Milling outer contour with 3mm endmill.


  1. Milling inner contours with 1/16" endmill.
  2. Toolchange
  3. Drilling with 3mm endmill.
  4. Milling outer contour with 3mm endmill.

Multiple designs with single job

If same thickness material is used for different designs or same design needs to milled out multiple times, then it is possible to save time by creating an assembly from those designs and single CAM job for the entire assembly. Parts should be placed flat next to each other with enough space between them that tool used for outer contour fits between them. For example when using 3 mm endmill, there should be at least 3 mm of space between parts to avoid cutting into the part next to the one being milled.

Personaalsed tööriistad