CNC Simulator Pro

user guide
×
Menu
Index

12.3.2. Tutorial 2 Milling

In this comprehensive tutorial, we'll delve into the world of milling with a focus on how to handle geometrically challenging parts using SimCam's mathematical capabilities. The tutorial will take you step by step through the process of creating a complex part with varying arc radii and centers. Along the way, we'll cover a range of topics such as setting up the workpiece, adding guide lines, points, and arcs, offsetting contours, and adding toolpaths (CAM).
 
This exercise is designed to enhance your understanding of milling processes and CNC programming, and to highlight the powerful functionality of SimCam. Whether you're a seasoned machinist looking to sharpen your skills or a novice seeking to gain a solid foundation, this tutorial offers valuable insights and hands-on experience. Let's dive in!
 
Our target component for this tutorial looks like this:
 
The dimension of the workpiece is X140, Y100, and Z30 millimeters. The part consists of several arcs with known and unknown centers and given radii. But with SimCam, this ambiguity is not a problem!
 
This tutorial is conducted in millimeters. Navigate to Program Settings under Settings, select the Program tab, choose 'Use millimeters', and confirm with the OK button. Then load the Milling Center machine by clicking this button and choosing from the Milling folder. Make sure to deselect the 'Load example' checkbox.
 
 
Our initial task is to ensure that our workpiece in the registry matches the drawing.
 
Navigate to SettingsInventory (F2) and select the Mill Workpieces tab. Add a new workpiece by clicking on 'Add New'.
 
 
Specify the dimensions X140, Y100, and Z30, assign a name to the workpiece, and close the window.
 
Well done! Now, let's incorporate the workpiece into the drawing.
 
Switch your view to SimCam by clicking the SimCam tab. From the SimCam menu, navigate to [More] – [Workpiece] and select the workpiece you've just created.
 
 
A rectangle representing your workpiece should now be visible on your screen. Use your mouse wheel to zoom out to a comfortable viewing level.
 
 
In case your workpiece is offset from the zero point, as shown in the image, follow these steps: Select [Modify] - [Move] from the menu after clicking on the workpiece border. Then click on the lower-left corner of the workpiece and the zero point to reposition it.
 
When you hover your mouse over the screen objects, information about them will pop up. Your mouse will “snap” to intersections, points, circle centers, and more.
 
The checkboxes below the SimCam screen let you control what the mouse should snap to.
 
 
Ensure that at least Endpoint (End), Center point (Cen), Intersection (Int), Extreme point (Ext), and Angle snap (Ang) are checked.
 
Time to begin drawing!
 
First, add some guide lines and points to simplify drawing the final geometry. Start by adding guide lines along the workpiece as shown below:
 
 
 
According to the drawing at the top, the center of the radius 28 is at X38 and Y50. Draw a point there by clicking [Point] - [Enter coords]. Enter 38 and 50, and click OK.
 
 
Using the same technique, add two more points, which are the centers for the two radius 16 to the right: X115, Y75, and X115, Y25.
 
 
Now let's draw the actual arcs.
 
Select [Circle/ Arc] - [Drawing Circle/ Arc] - [Center - Radius]. Click on the left point and drag the mouse until you see R:28.
 
 
For now, we're going to estimate the start and end angle; we'll fine-tune them later. Click somewhere near 25 degrees.
 
 
Move your mouse to somewhere near 330 degrees, press the space bar on your keyboard until the ghost arc looks like the image below, and then left-click your mouse.
 
 
Repeat this process with the two right arcs, radius 16. Ensure the angles make the arcs open up to the left.
 
Your component should look something like this:
 
 
Now, let's add the two arcs with unknown centers: radius 56 and 38.
 
From the SimCam menu, select [Circle/ Arc] - [Drawing Circle/ Arc] - [Two or three points].
 
Start by clicking ON the left arc for your first point.
 
 
For the next point, click on the top right arc.
 
Move the mouse until you see R:56.
 
 
Click there, then move the mouse to the intersection/tangent point on the left arc. The mouse should snap there. If it doesn't, ensure that Intersection (Int) snap is activated in the checkboxes at the bottom of the SimCam screen.
 
 
Move the mouse to the intersection/tangent point on the right arc, hit the space bar to see the correct ghost arc (as shown in the picture), and make another click.
 
 
Repeat this procedure for the radius 38 to the right.
 
Your drawing should now look like this:
 
 
Now let's add the bottom line. Select [Line] - [Drawing Line] and click ON the left arc and the bottom-right arc.
 
 
The next step involves adjusting the start and end angles for the arcs. Activate the left arc by clicking on it.
 
 
Drag the endpoint handles until they align near the intersection/tangent snap point and release.
 
 
Repeat this for all arcs and endpoints. Your component should now look like this:
 
 
Hovering the mouse over one of the arcs with an unknown center reveals that SimCam has calculated it for us.
 
 
SimCam is quite the mathematician!
 
The drawing above shows an inner contour offset by 10 mm. Let's add that using the offset function.
 
Select [Modify] - [Offset], then click on [Distance] and enter 10. Click OK.
 
 
Now, click on an object and then on the inside (near the object). Repeat this for each object along the contour.
 
 
At this point, if you wish, you can add dimensions using the Dimension menu selection. We recommend adding them on a separate layer, so they can be hidden while working on adding toolpaths (CAM).
 
Now would be a good time to save your drawing. Select FileSave SimCam file from the main menu, give it a name, and click OK.
 
Now for the fun part! Let's create a contour for generating the CNC codes.
 
From the SimCam menu, select [More] – [Contour] - [Track] and click the intersection as shown in the picture to set a start point for the contour.
 
 
Now the 'Tracker' will appear. It will follow your steps until you complete the contour. To guide the tracker, click on as many snap points along the way as possible.
 
 
Note! If the tracker veers off in the wrong direction, you can make it return by pressing Control - Z (Undo) on the keyboard.
 
To end the tracking function, hit ESC on the keyboard or right-click with the mouse.
 
Your component should now look like this:
 
 
Now it's time to set the parameters for the contour layer.
 
Click on the button at the lower-left corner to display the layers dialog.
 
As you can see, two layers have been automatically created for us: one guide layer and one contour layer.
 
 
Each layer's thumbnail on the left represents the objects on 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 appear.
 
At the top, enter the name of the operation and select the operation type. We will use this contour to pocket mill the inside.
 
 
For now, we can leave all other parameters as they are. Click OK to close the dialog.
 
As you can see, the pocket cuts have been automatically calculated for us, and a CNC program has already been generated!
 
 
One detail to note: the cuts, as you can see, go along the center of the contour. We need to correct this.
Disable the guide layer by clicking the Padlock button once, so it becomes locked.
 
 
Click on the contour to display its context menu.
 
 
Click on [Flip toolside] until the cuts appear on the inside.
 
 
Notice the small orange arrows pointing perpendicularly from the contour. These indicate the contour's "toolside". It can be either outside, inside, or on the contour (no arrows).
 
Now, look at the drawing again. We should have a 10 mm thick wall outside the inner pocket. Let's achieve this by setting the value of 'Save for fine cut' to 10 in the parameters.
 
Click the gear button again on the contour layer to display 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 the simulation will start.
 
 
Now we will add contours to make an outside pocket operation to remove the rest of the material.
 
Click on the SimCam tab to return to the SimCam view.
 
Click on the padlock on the guide layer to enable it and on the eye button on the contour layer to hide it. Make sure the guide layer is the selected layer (indicated by a grey frame around the layer).
 
 
We will define a new contour around the workpiece borders using the same technique as before.
From the SimCam menu, select [More] – [Contour] - [Track].
 
Click the lower-left corner of the workpiece rectangle, then the upper-left corner, followed by the rest to end the contour. End by hitting ESC on the keyboard.
 
Important! Every time we create a new contour, a new contour layer will be added automatically if a guide layer is the selected layer. The selected layer has a grey frame around the layer. As we are going to create a pocket with an island, we need more than one contour on the same layer, so we need to select the contour layer to prevent the 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.
 
Your layers and drawing should now look like this:
 
 
The third and final layer contains two contours. The second and subsequent contours will automatically be treated as islands when we create a pocket layer.
 
Click on the inner contour and select 'Flip toolside' twice so that the small directional arrows are pointing outwards, meaning that the toolside is on the outside of the contour.
 
The final step is to set the parameters for this layer as well. 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 generate CNC code.
 
Now you should see this:
 
 
Click the play button again to simulate the result.
 
 
 
Excellent work!
 
Now, feel free to experiment with the parameters to customize the output. Try to add drilling, stepping, and ramping operations. Always remember, the goal is to learn and have fun!
 
That concludes our milling tutorial using SimCam. Hopefully, this exercise has provided you with a strong understanding of how to utilize SimCam’s mathematical capabilities to handle geometrically complex parts. By following these steps and experimenting on your own, you can gain a deeper understanding of milling processes and CNC programming.
 
Remember, the more you practice and play around with the software, the better you'll become at visualizing and executing your designs. Don't be afraid to experiment and try new things; that's how great ideas are born!
 
Thank you for joining us in this exercise. We hope you found it informative and engaging. Stay tuned for more tutorials and exercises to further your knowledge in this exciting field! Keep milling and keep learning!