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:
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 Settings – Inventory 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 screen size 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 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 End point (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 point. They will make it easier for us to draw the final geometry.
From the drawing abowe, 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.
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:
Repeat this procedure with the two arcs radius 16 to the right, this time make sure you have the angles so that the arc opens up to the right.
Now 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.
The next click on the top right arc.
Move the mouse until you see R:56.
Click there and move the mouse 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 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.
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 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 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 to 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 File – Save 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 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.
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 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.
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.
Click on the eye button on both layers to show the guide layer and hide the contour layer.
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 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.
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.
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!