Valid for version 220.127.116.11 and later. This tutorial is made for the Turning Center machine set to millimeters.
Part one: Basic operation for external turning.
Load the machine and make sure you have millimeters selected as units in settings.
Now we will create a workpiece to use in the tutorial.
Press the F2 key to open the Inventory Browser and click on the Lathe Workpieces tab.
Click on the "Add" button and enter the name "Tutorial Part" and the Diameter 70, Length 100. Do not select a material as the default Aluminum material will be used.
Click on OK to close the Inventory Browser.
Click on the SimCam tab to view the SimCam window.
Click on "More" - "Workpiece" in the SimCam menu and browse to the workpiece we have just created. Click on OK to insert it in our document.
Now we are going to add a roughing layer and draw a contour for the shape of the final workpiece.
Click on the Layers button in the lower left corner of the SimCam Window to view the Layers panel.
Let us first go through the most important things on the layers panel.
These three buttons are the most important to know. You use the refresh button as soon as you want to update the thumbnail images as well as the CNC code with the latest changes. The gear button to the right in the layers panel toolbar is used to create new operation layers and finally, the gear button at each layer is used to open the parameters for that operation layer. Please also note that you can open the parameters for the layer by double clicking the cyan colored information box at the layer.
Another handy trick to know is that you can hold down CTRL on the keyboard and click the cyan colored box to make that layer the only selected and visible one. Try it out!
OK, let's continue:
Click on the gear button at the bottom of the layers panel and select Roughing from the popup menu.
You should now see two layers in the layers panel.
Close the layers panel or move it out of the way for now.
From the toolbar at the bottom of the SimCam window, click on the grid snap button and select 1.
Click "More" - "Contour" - "Follow mouse" in the SimCam menu.
Move the mouse to X0 Z98 and click for the start point. Zoom in if needed.
Move the mouse straight up to X30 and make the next click.
Move the mouse straight to the left to Z80 and click.
Continue by clicking at the following coordinates:
To end the contour, make a right click with the mouse or hit ESC on the keyboard.
This is how your drawing should look like.
No zoom in on the corner at X26, Z60 and click on the contour. Click "Modify" - "Fillet" and enter 10 in the value box shown at the bottom of the window. Finally press Enter.
Now, do the same thing at the X60 Z60 corner, this time selecting "Chamfer" from the "Modify" menu. Enter 2 and press Enter.
This is how your drawing should look like, please notice the automatically created ghost line that helps you see the contour as a drawing part.
It is a good time to save the drawing now. From the main menu, select "Save SimCam File" and enter a name for the drawing, for example SimCamTurningTutorial1.
OK, good work! Now, let's start cutting!
At the bottom of the layers panel, click the leftmost button (refresh) to create the CNC code from the drawing. Remember that you should always click this button when you want to force SimCam to recreate the CNC code.
As you can see in the editor window, there was not much of a CNC program created. Also the roughing layer turned red/pink to notify you that there is a problem. Don't worry, it is normal. If you click the information button on the layer, you will see that SimCam is missing two points on the layer to define the workspace.
The two corner points of the workspace tells SimCam where you want to start cutting and where you want to end. Let us add the points now.
From the SimCam menu, select "Point" and then click at X68 Z102.
You will see an orange point indicating the start point of the workspace.
Make another click at X26 Z10.
Click the refresh button at the bottom of the layers panel.
We got cuts created, but something is not as it should!
As you can see, the cuts do not stop at the contour. They all go to the end point of the workspace.
This is because we have not decided the toolside of the contour yet. If you look closely there are small arrows pointing out from the contour.
They point to the left side by default. In our case, we need them to point to the right side of the contour so that SimCam understands that it is where we want the cuts to stop.
Click on the contour and select "Flip toolside" from the menu.
Click two times so that the arrows point to the right of the contour.
Note how the cuts change, they now stop at the contour. Always remember to set the toolside correctly on all contours.
Let's change the depth of cut to a slightly smaller value.
Double click on the cyan colored box on the layer, or click on the gear button to open the parameters for the operation.
Set the Depth of Cut parameter to 3 mm.
Click OK to close the parameters and see the result on the cuts.
Now we will add a facing operation.
At the bottom of the layers panel, click on the gear button and select Facing.
The Facing operation needs a workspace just like with Roughing. Select "Point" from the SimCam menu and make the first click at X32 Z100 and the second click at X-2 Z98. This gives us a millimeter of overcut.
Note! If you have problems clicking coordinates because the mouse snaps to other objects, make the other layers inactive (and invisible if you want). If you hold down the CTRL key on the keyboard while clicking on the cyan colored box on a layer, that layer will become the only visible and selected layer in the document.
Now open the parameters for the new layer and select tool number 27 (make sure to check the "Use Embedded tool" checkbox).
Set 1 mm for depth of cut this time.
Info! Tools in the browser are drawn with the insert at the top. In machines where the tool holder points upwards (like the Turning Center) the tool simply gets mirrored around the Z axis. This is automatically handled by the CNCSimulator so that we do not have to draw two of each tool.
Close the parameters by clicking OK and look at the result.
Click on the Play button to simulate the work we have made so far.
Press CTRL - S on the keyboard to save the SimCam drawing at this stage.
Let us now add a finishing cut.
Click on the gear button at the bottom of the layers panel and select "Finishing" from the popup menu.
Add a point at X68 Z99.
Add another point at X26 Z40.
Open the parameters for the new layer and select embedded tool number 28.
Click OK to close the parameters. Still no finishing cut will be created. This is because we need the contour on this layer as well.
Click on the contour and select "Copy" from the menu. Make sure the contour layer is enabled.
Click on the thumbnail image of the Finishing layer to make sure it becomes the selected layer.
The selected layer has a dark gray background.
From the SimCam menu, select "More" - "Paste" to insert the copied contour on the Finishing layer.
Click the refresh button at the bottom of the Layers Panel to recreate the CNC code.
Press CTRL - S to save, then click on the play button to simulate the part.
Before, after or during simulation, click on the little knife button at the bottom of the simulation screen and check the "Show inside" checkbox. This is how the part should look now.
This concludes the first part of the tutorial. You can now choose to play around with SimCam on your own before doing part two, or to directly continue by reading on.
Part 2: Adding drilling and threading operations.
Welcome back! Let's drill a hole in the workpiece.
Add a drilling operation layer to the document.
Open the parameters for the layer and select the embedded tool number 17. Then click on the Drilling tab and enter 70 for "Drill to Z".
Click OK to close the parameters and select "Point" from the SimCam menu.
Click at X0 Z100.
Click the refresh button at the bottom of the Layers Panel to recreate the CNC code.
Save the drawing and simulate again to check what we have done so far.
Congratulations! One operation left to go!
Add a Threading layer to the document.
Add two points for the threading workspace. The first point at X30 Z98 and the second point at X26 Z79.
Open the parameters for the layer and select the embedded tool number 25.
For the threads to look nice when simulating, we need to boost up the resolution temporarily. You can add the special command $OverrideBufferQualitySetting 8 to the very top of the CNC code to get a better resolution (and slower simulation speed).
Please note as soon as you refresh the program, SimCam will overwrite your manual change in the CNC code, so the $Override... command will go away.
Great! This concludes part 2 and the tutorial. We have showed you how to use common operations. As you have noticed, we did not focus too much on cutting parameters and mostly accepted the default ones in this tutorial.
Now, try to do your own first work using the methods we have showed you here.