FablabSU

Go to Windows Start menu and Open “Galaad (fraisage), note the Blue Icon

This is the main page of the Galaad Interface. It should appear blank, however if the previous user did not save/quit their work, another job maybe loaded onto the White workspace. Either way, the procedure will be the same.

Select “Fichier” (Files) and the scroll down to “Import” and select your project. See here for accepted file formats.

After your project has been selected, the “Import menu” will appear. This menu will allow you to rescale your project if desired. In most cases, we can leave the menu exactly “as is” and select “OK”.

In the case that a .DXF is used:

After selecting “OK”, a 2nd and final “import menu” will appear asking if you would like to convert to .dwg Click Non

The Project has now been imported, but the dimensions of the stock material is too small. Select Fichier (File), then scroll down to “Dimensions Brute” (Stock Dimensions)

The “Stock Material” Menu will load and here we must insert our XYZ dimensions, aquired from Step 1 in the tutorial. Then Select OK

The “Select” tool can also be used to select individual features in the design.

Now that the Stock material has been increased to a proper size (with a small margin concerning X and Y), we can use “Ctrl-A” to select all and reposition the project in the work zone. Allow for a small margin of error on the left and bottom dimension.

Using the “select tool”, highlight the first inner pocket to be milled (shown in photo). Then select “Depth/Speed/Tool Menu”. For a more indepth understanding of this menu, see here.

In this example, we will be using:

• Depth: 1.3mm
• Speed: 9mm/s (However, after further testing, I would advise a lower speed of 5mm/s
• Tool: 3mm flat end-mill

• *Click OK You are brought back to the workspace. Now we must hover over the “Hatching” menu until the “Pocket” menu appears. Select “Pocket” In this example we will be using: * Distance between passes: 1.25mm * Progession: 0 * Direction: Clockwise * Angles: Rolling * Avoid inside islands: NO * Connect neighboring passes: NO For a more indepth understanding of this menu, see here. Click OK We can now see the new created “Tool Path” for our 3mm flat end-mill. We see that it will create a spiral patern working its way from the center to the contour of our defined Pocket. Next, we will select all 6 of the small (5mm) holes that must be pierced into this part. Select the “Depth/Speed/Tool Menu” In this example we will use: * Depth: Cut-off * Speed: 5mm/s * Tool: 3mm flat end-mill For a more indepth understanding of this menu, see here. Click OK We are brought back to our workspace, DO NOT UNSELECT THE 6 CIRCLE CONTOURS. Since these are destined to be screw-holes, the inside diameter is very important. We must selec the “Contouring Menu”. A more in depth explination of this menu can be had here. However, for this example we will be using the parameters: * Trajectory: Interieur * Angles: Roll over the angles * Ebauche: Empty * Direction: Clockwise * Over-pass: Empty Select OK We are brought back to the project workspace. We can now see our newly generated tool-paths indicating that the tool will in fact cut on the interieur of our designed contour. We will now select the 4 larger circles (12mm). These are destined to be counterbores for some anchor screws. Then select “Depth/Speed/Tool Menu”, in this example we will be using the parameters: * Depth: 10mm * Speed: 5mm/s * Tool: 3mm Flat end-mill Click OK After being brought back to the project work space, WHILE THE COUNTOURS ARE STILL SELECTED, select the Pocket Tool. In this example we will be using the parameters: * Distance between passes: 1.25mm * Progression:0mm * Direction: Clock-wise * Angles: Rolled * Sequence: From Center to contour * Avoid internal islands: NO * Connect neighboring passes: NO Click OK As before we will notice the new tool path created on the inside of our 12mm Counter bores. * NOTE- We intentionally chose the order of operations as “Contour” then “Pocket”, as it is clear that a precise selection of the inside 5mm screw holes is impossible with the new “Pocket Toolpath”. We will now select the outter contour of our project. It is important that there is a small margin of error given to the Left and Bottom. To understand why, see here. Select “Depth/Speed/Tool” Parameters: * Depth: Cut off * Speed: 3mm/s (this is slower than the others as the tool will be cutting from both sides of the tool at all times and will create “chatter” if the speed is too high. * Tool: 3mm Flat End-mill Click OK After we are brought back to the Project Work Space, we must select the “Contouring Menu” while the exterior contour is still selected. When the Contour Menu Opens we will use the parameters: * Trajectory: Exterieur * Angles: Roll over the angles * Ebauche: Empty * Direction: Clockwise * Over-pass: Empty**

Finally we have all of our tool-paths defined for all of the features of our Project. We can select any of the given toolpaths/contours and reselect “Depth/Speed/tool” if we chose to make any modifications.

On the contrary, if we wish to change our contours to “exterior or interior” we must delete the given tool-path that we wish to change and re-create a new one. This is the same for pockets/hachuring.

Now that the toolpaths are defined, we must only select the “Machine” Icon. This will launch the Galaad Machining interface.

Your project has now succesfully been imported into Galaad Machine Interface. You are now only moments away from maching your project.

To understand the Galaad Machine Interface and material set up, I advise that you procede to. Step 4 of this tutorial.

Table of Contents