face operation freecad

Face Operation – FreeCAD Path #7

Facing – FreeCAD Path

We begin the machining of this part with the Facing operation and with this operation we remove the allowance at the top of the material.

After selecting this operation window shown below could appear.

Select the tool and click OK.

On the left we have a window with the parameters definition for this operation.

Operation Tab

And by default the Operation tab opens.

In the Tool Controller parameter we specify the tool we will use to perform this operation. Here we choose T11 Flat 10.

The Boundary Shape parameter defines the machining boundary. And we have three options to choose from. Perimeter, Boundbox and Stock. Let’s leave the default parameter for now, and then we’ll change individual parameters and check how the tool path changes.

In the Cut Mode parameter we specify the milling method. Climb or Conventional.

As for the Pattern parameter, this is how the toolpaths will be generated, what their shape will be.

The Angle parameter specifies the angle of the tool paths relative to the X axis.

The Step Over Percent parameter is the value of the overlap of successive tool path passes. Expressed as a percentage of the tool diameter.

And the Material Allowance parameter is the allowance we leave after this machining.

For now, let’s leave the default parameters here, later we will change them and check how the tool path changes.

Let’s check the other tabs. And here we will start to change something and check how the tool path will change and finally we will return to the Operation tab, because there are the most parameters to discuss.


Base Geometry Tab

In the Base Geometry tab we specify the geometries to be machined. This is not necessary for facing, so we can leave it empty. Or we can indicate the top wall of the model.

First select the wall and then click the Add button.

To remove any geometry, in case we select too much, select the geometry in the list and click Remove. To remove all geometries, click the Clear button.

Ok, let’s add the top face of the model as the geometry to be machined and click OK to calculate the tool path.

And now it may turn out that this path will be invisible, but this does not mean that it is not there.

It was covered by a part model. But why did this happen?


Toggle Visibility

At this point, one more thing needs to be clarified. The 3D model on the basis of which we prepare the machining is a copy of the model from the Part or Part Design workspace.

So starting the CAM project, the 3D model was copied to this project and based on this copy we prepare the toolpaths. Okay, but that still doesn’t explain why these paths are invisible.

Let’s move to the Combo View and here we have the Body part, which is what was created in the Part Design workspace and we also have a CAM project called Operation 1.

And now when you look at the CAM project we have a Model tab, in which we have a Model-Body, but it is grayed out.

Right click on this model and choose Toggle visibility.

And as you can see in the work area a second model has appeared and this is the model on the basis of which we created the toolpaths.

So, in the workspace, a model from the Part Design space has been displayed so far.

And as you can see they are shifted relative to each other, and this is because for the model in the CAM project we changed the origin of the coordinate system.

To make everything ok, all you have to do is hide this model by right clicking and choosing Toggle visibility for model from Part Body.

And now the workspace will display the model from the CAM project called Operation 1 and the toolpath.

It is worth remembering this because at the beginning of work with the FreeCAD CAM module it may seem to us that something is wrong with this system. But everything is all right, and after having completed several CAM projects, it will start to make sense that a copy of the model for the CAM project is being created.

Ok, let’s discuss another parameters.


Change the operation name

But by the way, let’s change the name of this operation. We don’t have to do this, but it’s worth knowing this option.

Right click on the operation and choose Rename or simply click F2 on the keyboard.

And enter the name 1-Face.

Now edit this operation by double-clicking the left mouse button on the name of the operation (or right click and select Edit).


Depths Tab

And let’s go to the Depths tab. The Depths tab defines the machining levels.

The Start Depth level determines the upper level of machining, the top of the material. The value is empty because it is automatically read as the top of the stock.

When you click the left mouse button on the icon next to the value, a window will appear in which this value is specified by a variable and in this case it is OpStartDepth.

We can change this value. E.g. Adding + 1mm or simply entering a value.

Click OK.

Before accepting the changes, let’s check what the toolpath looks like.

We see that there is one pass in the Z axis on the top of the model.

Click the Apply button to accept the changes and you won’t see any changes.

This is because the step value in Z is determined by the Step Down parameter and it is 10 mm.

And the value of the final depth, determined by the Final Depth parameter, is -1 mm.

So the distance from the initial level specified on Z1 to the final machining level specified on Z-1 is 2 mm, which is less than the maximum value of one pass in the Z axis (set to 10 mm).

If we now change the Step Down value to 1 mm and click the Apply button, the changes will be noticeable.
Two Z-axis passes with 1 mm each will be generated.

So, the initial machining level is the value in Z1, the step down is 1 mm, so the first pass will be generated at the coordinate Z0.

The final machining level is the Z-1 value, so between Z0 and Z-1 we have 1 mm, which is the value of the step down, so there is material left for one pass and the second pass will be generated at the Z-1 coordinate.

But how did it happen that the first pass was generated at the Z0 coordinate, as soon as the material begins there?

Whatsmore we even defined the stock so that we have only 1 mm allowance at the top of the part.

And as you remember by default this level, level Z0, has been read to the Start Depth parameter, i.e. to the initial level of machining.

But in this tab we can fool it a little and start machining a little above the material.

In the same way we will be able to change the final level of machining, which will be useful in machining contours and we will come back to it.

In the Depths tab we have another parameter, the Final Depth parameter, and it indicates the value of the finishing pass. And what exactly does this mean? Let’s check the example.

Let’s change this value to 0.2 mm and click Apply.

And as you can see there is a third pass in the Z axis. And the distance between the second and third pass is 0.2 mm, which is the value as we set in the Final Depth parameter and this is the finishing pass. Simply, we leave a small layer of material on the last pass to get a better surface finish.

And so, the first pass will be at the Z0 coordinate, the second pass will be at the Z-0.8 coordinate and the third pass will be at the Z-1 coordinate.

This is quite a useful parameter.


Heights Tab

Ok, let’s go to the Heights tab.

Here we have two parameters Safe Height and Clearance Height.

The Clearance Height level defines the safe level above which the tool can move quickly without risk of collision with the fixings.

And the Safe Height level means the level to which the tool will go down quickly in the Z axis after it is set in the XY coordinates of the start of machining, at the Clearance Height level.

So, first the tool, with a rapid movement of G0, at the Clearance Height level moves to the XY coordinates of the beginning of machining, and then with a rapid movement in the Z axis it goes down to the Safe Height level and from this level it starts working with the feed rate G1.

Later, if we have more than one operation, we will analyze at what level the tool moves between operations.

We will return to the Operation tab in a moment, but first let’s analyze the machining program.


Similar Posts