In this tutorial, we are going to use the Polar Coordinates Calculator, the Arc Calculator, and the Corner tool. You find them all under Tools - Helpers in the menu.
This tutorial is made in millimeters. Open a milling machine and change the settings to millimeters if it is not already set.
Consider the drawing below. We have many dimensions on it, but not all positions are there. They have to be calculated. For example, we have no idea where the 69.469 distance angled line ends in the X-axis and we also do not know where the center of R16.071 is located.
We could, of course, draw the contour in SimCam and have it creating the CNC program for us, but there is an alternative method using the built-in helpers.
We are only going to focus on solving the unknown coordinates, in this exercise. If you would do this as a real project, you would need to add roughing cuts, as well as radius compensation (G41/ G42) and realistic feeds and speeds.
Start by adding a workpiece with the size X100, Y80, and Z25.
Click on the "Insert at cursor" button.
Let us now move the zero point of the program to X5, Y6.867, and Z25, to make it easier to create the program (the dimensions are drawn from that position). We also select a tool.
And then we add a couple of blocks, to position the tool and feed down to Z-5.
Now, let us have a look at the drawing again.
Our first position is easy, it is located at X0, Y25.517 according to the drawing. We add this to the program.
Now it's getting trickier. We don't know where the next position is. Let us use the Polar Coordinate Calculator.
First, simulate the program you have so far. This will help us as the reference point will be filled out automatically from the current tool position.
Click on Tools - Helpers - Polar coords calculator or press Control - O on the keyboard.
The angle is 123.1 according to the drawing, but we measure the angle from straight to the right, so we will have to take 90 degrees off that value. We end up with 123.1 - 90 = 33.1 degrees.
The distance is 69.469 according to the drawing.
As you can see, the calculator creates the CNC block for us. Click on the "Insert at cursor" button to send it to the program.
Simulate the program again.
Great! Next, let us do the arc in the corner.
The corner tool can help us with all three blocks to go over the corner and end at the beginning of arc R16.071.
Click on Tools - Helpers - Corner fillet or chamfer.
As you can see from the hint picture in the dialog, we need to type in 3 points. The first one is already filled in for us as it is the current tool position. The second one is the position of the corner and then the endpoint.
The final position in Y, is not written on the drawing. But we can easily calculate it by taking 17.026 from our current position. We end up with 63.454 - 17.026 = 46.428.
We also type in the radius (10) and our blocks get automatically created for us.
Again, click the "Insert at cursor" button.
Simulate the program.
Now it is time to deal with the arc (R16.071) on the right side. From the drawing, we see that we know its endpoint but we do not have any information about its center. Let us use the Arc Calculator to solve that problem.
Click Tools - Helpers - Arc Calculator (or press Control - R on the keyboard).
The start point has already been filled out for us. Enter the endpoint and the radius and put the switch in the Anti-clockwise direction.
Again, click "Insert at cursor".
Now, add the remaining blocks to go back to the start of the contour.
We hope that this tutorial has shown you how easy it is to solve geometrical problems using the Helpers.