CNCSimulator Pro

user guide
Index Tutorial 2 Milling

Important note: This tutorial was written prior to version 2.5. Earlier versions did not have CAD drawing lines, arcs and circles. Because of this we are only using basic guide lines and circles here. For updated tutorials, look under the topic "Version 2.5 and later".
In this exercise, we are going to manufacture a geometrically challenging part with unknown points to put SimCam’s mathematical skills to a test.
Here is a video of the steps in the tutorial. Use it as a companion (pause and play as needed) during the tutorial.
This is the part we are going to do in this exercise:
Size of the workpiece is X140, Y100 and Z30 millimeters.
As you can see, we know the center of some of the arcs but not all. Other arcs just have a known radius. For SimCam, this is not a problem!
The tutorial is made for millimeters. First go to the Program Settings by selecting Settings - Settings  and choose the Program tab. Select Use millimeters and click on the OK button. Then load the machine by clicking this button and select the Milling Center machine. Do not forget to uncheck the Open demo checkbox.
The next thing we have to do is make sure we have a workpiece matching the drawing in our workpiece registry.
Click SettingsInventory Browser (F2) in the main menu and select the Mill Workpieces tab.
Now, click on the green plus button in the upper right corner to add a new workpiece.
Enter X140, Y100 and Z30 and type in a name for the workpiece, then click OK.
Great! Now let's start by adding the workpiece to the drawing.
Click the SimCam tab to switch view to SimCam.
From the SimCam menu, click [More] – [Workpiece] in the menu and select the workpiece created above.
You should now see a blue rectangle representing the workpiece on screen. With the mouse wheel, you can zoom out to a screen size you like.
SimCam uses so called Guides Lines and Circles to define the geometry. As you can see, four guide lines have already been added for you. SimCam has also added some useful points.
When you move the mouse over the objects on the screen, you will see information about them and the mouse will “snap” to intersections, points, circle centers, etc.
As you can see from the drawing, there are certain key measurements we can use to draw our geometry. Here they are marked by red lines. Let's start by drawing them with guide lines.
To put vertical lines at 38 and 115, we can use the offset function to make offset copies of one of the guide lines automatically created when we added the workpiece.
From the SimCam menu, click [Offset].
Click on [Distance] and enter 38.
Click on the vertical line at the left side of the workpiece.
Click somewhere to the right of the line to create an offset copy at the distance 38.
Click [Distance] again and enter 115 this time. Repeat the procedure to create an offset copy at the distance 115.
Now, use the same technique to make horizontal offset copies from the bottom line at Y 25, 50 and 75.
Result when all guide lines are in place.
Next step will be to add guide circles in the intersections between the lines. To the left we add a circle with radius 28 and to the right we add two circles with radius 16.
From the SimCam menu, click [Circle] – [Center – Radius].
Hover the mouse cursor over the center left intersection and note how the hair cross snaps to the point when you get near (snap points has gravity).
Click once to fix the circle center point.
Now, drag the mouse until you read 28 for its radius and click one more time.
If you hold the mouse over the circle, this is what you should see.
The X and Y coordinates are 20 mm larger than might be expected but this is because we accepted the default X20, Y20 workpiece offset when we added it.
Now, repeat the steps to add the two radius 16 circles to the right. Now your drawing should look like this:
Look at the drawing at the beginning of the tutorial. As you can see we have a tangential arc of radius 56 at the top and another on of radius 38 to the right. We do not know the center nor the start and end point of these arcs. To draw them, we have to use the other circle drawing function.
From the SimCam menu, click [Circle] – [Two or three points].
Click on the left circle (be careful not to click on a snap point but rather directly on the circle border). Be careful to click near where you think the arc will tangent.
Click on the upper right circle.
Drag the mouse until you read 56 for the radius, make a final click.
Repeat the steps to draw the radius 38 circle to the right.
Please note that you can type in the radius as well. You do that by clicking [Enter radius] in the SimCam menu.
Final step to complete our guides is to add the straight line that tangents to lower circles.
From the SimCam menu, click [Line].
Click on the first and second circle just as you did when drawing the tangential circles. Be careful to click on the object itself and not on a snap point, zoom in if necessary.
Now your drawing should look like this:
It is a good time to save the drawing now. Click FileSave SimCam file from the main menu. Type a name and click OK.
Now comes the fun part! Let's add a contour that will be used for creating the CNC codes.
From the SimCam menu, click [More] – [Contour].
Click the lower right intersection to set a start point for the contour.
Now you will see “the Tracker”. He will follow your steps until you are done with the contour. To show the tracker where to go, click on as many snap points along the way as possible.
When you are done, your drawing should look like this.
When you reach the last point (8) do a final click and then click on [Done] in the SimCam menu.
Your drawing should now look like this:
It is time to set the parameters for the contour layer.
Click on the button at the lower left corner to show the layers dialog.
As you can see, two layers have been automatically created for us. One guide layer and one contour layer.
To the left on each layer, you see a thumbnail presentation of the layer. At any time you can show/ hide and enable/ disable a layer. Each contour layer has a gear button to open its parameters.
On the contour layer, click the gear button.
The Cutting Operation Parameters dialog will be shown.
At the top, enter the name of the operation and select operation type. We will use this contour to pocket mill the inside.
For the moment, we can leave all other parameters as is. Click OK to close the dialog.
As you can see, the pocket cuts have been automatically calculated for us, and a CNC program is already produced!
One detail though, as you can see, the cuts goes on the outside of the contour. We need to correct that.
Disable the guide layer by clicking the Padlock button once so it becomes locked.
Now, click on the contour to show its context menu.
Click on [Flip toolside] until the cuts shows up on the inside.
Like this!
As you can see, there are small orange arrows pointing in the perpendicular direction from the contour. These show the contours "toolside”. It can be either outside, inside or on the contour (no arrows).
But hey, look at the drawing again! We should have a 10 mm thick wall outside the inner pocket. Let's do that by putting in value 10 as Save for fine cut in the parameters.
Click the gear button again on the contour layer to show the parameters dialog.
Type in 10 in Save for fine cut.
Click OK again and note the change in both the drawing and the CNC program.
At this point, we can check the CNC program by clicking the play button.
The view will automatically change to the 3D view and simulation will start.
Now we will add contours to make an outside pocket operation to take away the rest of the material.
Click on the SimCam tab to get back to the SimCam view.
Re-enable the guide layer and hide the contour layer for easier drawing.
We will define a new contour around the workpiece borders using the same technique as before.
From the SimCam menu, click [More] – [Contour].
Click the lower left corner of the workpiece rectangle and then the upper left corner followed by the rest to end the contour. Finally, click [Done].
Important! Every time we create a new contour a new contour layer will be added for us if a guide layer is the selected layer. The selected layer has a dark gray background. As we are going to make a pocket with an island, we need more than one contour on the same layer and hence we need to make the contour layer the selected one to avoid automatic creation of a new layer.
In the layers dialog, click the info panel of the contour we just created to select it.
Now we can define the second contour that will end up on the same layer. Define the contour with the arcs and line just as we did with the first contour.
Now your layers and drawing should look like this:
The third and final layer contains two contours. The second (and following) contour(s) will automatically be treated as an island(s) when we make it a pocket layer.
Now, disable the guide layer by clicking the Padlock button.
Click on the outer rectangular contour and select [Flip toolside] once so that the small directional arrows disappears meaning that the toolside is ON the contour.
Final step is to set the parameters for this layer too. Click on the gear button.
As before, type in the name of the operation and select pocket for the operation type.
Click OK to close the parameters dialog.
Make the second layer visible again by clicking the Eye button. Please note that only visible layers make CNC code.
Now you should see this:
Click the play button again to simulate the result.
Great job!
Now, feel free to experiment with the parameters to customize the output. Try to add drilling, stepping and ramping operations. And remember to have fun!