CNCSimulator Pro

user guide

12.3.2. Tutorial 2 Milling

In this exercise, we are going to manufacture a geometrically challenging part with unknown points to put SimCam’s mathematical skills to a test.
This is the part we are going to do in this exercise:
The 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 in the folder Milling. 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 rectangle representing the workpiece on screen. With the mouse wheel, you can zoom out to a level you like.
If your workpiece ended up offset from the zero point, like in the picture, do the following:
Click on the workpiece border and select [Modify] - [Move] from the menu. Then click on the lower-left corner of the workpiece and thereafter the zero point to move the workpiece there.
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.
You control what the mouse should snap to using the checkboxes below the SimCam screen.
Make sure you at least have Endpoint (End), Center point (Cen), Intersection (Int) Extreme point (Ext) and Angle snap (Ang) checked.
Let's start drawing!
We can start by adding some helper guide lines and points. They will make it easier for us to draw the final geometry.
Start to add guide lines along the workpiece as shown below:
From the drawing, at the top, we can see that the radius 28 has its center in X38 and Y50. Let us draw a point there. Click [Point] - [Enter coords]. Enter 38 and 50 and click OK.
Now add two more points using the same technique. They are the centers for the two radius 16 to the right.
X115, Y75 and X115, Y25.
Now let us add the actual arcs.
Click [Circle/ Arc] - [Drawing Circle/ Arc] - [Center - Radius].
Click on the left point and drag the mouse until you see R:28.
We are going to estimate the start and end angle for now, they will be adjusted later. Click somewhere near 25 degrees.
Move the mouse to somewhere near 330 degrees and hit the space bar on the keyboard until the ghost arc looks like on the picture:
Left-click the mouse button.
Repeat this procedure with the two arcs, radius 16, to the right. This time make sure you have the angles so that the arcs opens up to the left.
Your part should look something like this:
Now, let us add the two arcs with unknown centers, radius 56 and 38.
Click [Circle/ Arc] - [Drawing Circle/ Arc] - [Two or three points] from the SimCam menu.
Make your first click ON the left arc.
Make the next click on the top right arc.
Move the mouse until you see R:56.
Click there and move the mouse to the intersection/ tangent point on the left arc. The mouse should snap there. If not, make sure you have Intersection (Int) snap 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 (like on the picture) and make another click.
Repeat this procedure for the radius 38 to the right.
You should now have:
Now we will add the bottom line. Click on [Line] - [Drawing Line].
Then click ON the left arc and the bottom-right arc.
The next step is to adjust the start and end angles for the arcs.
Click on the left arc to make it activated.
Click and drag the endpoint handles until they get near the intersection/ tangent snap point and release.
Repeat with all arcs and endpoints. Now your part should look like this:
If you hover the mouse over one of the arcs with an unknown center, you can see that SimCam has calculated it for us.
SimCam loves to do math!
As you can see from the drawing above, we have an inner contour that is offset 10 mm. Let us add that one using the offset function.
Click [Modify] - [Offset]. Then click on [Distance] and enter 10. Click on OK.
Now click on an object and then on the inside (near the object). Repeat for each object along the contour.
At this point, if you want, you can add dimensions using the Dimension menu selection.
If you choose to do so, we suggest you add them on a separate layer, so they can be hidden while working with adding toolpaths (CAM).
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] - [Track].
Click the intersection as on the picture to set a startpoint for the contour.
Now you will see “the Tracker”. It 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.
Note! If the tracker takes away in the wrong direction, you can always make it come back 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 part 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 representation of 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 be shown.
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 the moment, 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 is already produced!
One detail: as you can see, the cuts go on the center of the contour. We need to correct that.
Disable the guide layer by clicking the Padlock button once so it becomes locked.
Click on the contour to show its context menu.
Click on [Flip toolside] until the cuts show up on the inside.
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).
Now, 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 the 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.
Click on the padlock on the guide layer to enable it and on the eye button on the contour layer to hide it.
We will define a new contour around the workpiece borders using the same technique as before.
From the SimCam menu, click [More] – [Contour] - [Track].
Click the lower-left corner of the workpiece rectangle and 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 for us if a guide layer is the selected layer. The selected layer has a yellow background. As we are going to make a pocket with an island, we need more than one contour on the same layer, so we need to make the contour layer the selected one to avoid 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.
Now your layers and drawing should look like this:
The third and final layer contains two contours. The second and following contours will automatically be treated as islands when we make it 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 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!