Preparing files for the Maslow with VCarve Pro

Setting up the maslow as a machine

Use these settings for the Maslow as a machine. You need to do this so that tools setup for your machine are saved for the maslow, and not the ooznest.

Sheet setup

Use these settings on the left hand side to setup the work area. Choose your own sheet dimensions, sheet depth and material. We are using 9mm full sheet of MDF. There's no real reason not to use a full sheet. You must click OK before you can import.

XY datum position should be in the middle as that is the XY datum for the maslow & Z should be aligned on the surface of the material.

Importing DWG/SVG etc

Click the import option. If it is greyed out, it is because you have not clicked OK for the sheet material section.

Occasional errors

If you get this, ignore.

moving items

Use the transform items to centre your piece onto the material.

once imported, it'll look something like this, but with your design.

Show Toolpaths

Click "toolpaths" and select the "show toolpaths tab"

and select profile toolpath

Creating a toolpath

Check the cut depth is the same as your sheet.

Select the correct end mill, then click "edit tool"

The maslow takes 1/4, 8mm and 6mm bits (select the corect collet to use though!)

The above is for a 1/4" bit with a 1/4" shank using the 1/4" collet!

In tems of the spindle speed, this is not settable, so ignore.

Feed units mm/min Feed rate 600mm/min Plune rate 300mm/min

The pass depth should be half the cutting bit width. So for a 1/4" bit, which is 6.34mm, the cutting depth is 3mm (though it could be 3.17mm)

To cut through 9mm, you need to have 3 cutting passes of 3mm each. This may not cut all the way through and leave a paper thin layer. You may need a fourth or clean it up on the router table.

The above shows "Outside/right" "inside left" and "on"

Outside/right = cut on the outside of the line or to the right if it is a single line. Inside/left = cut "in" a line or to the left if it is a single line On = cut "on" the line - like a laser cutter.

If you were cutting out a shape, you'd most likely cut "outside" if you're cutting something out, like a hole for a button, you'd cut "inside".

You select the path it applies to by clicking with the mouse. If you click and only part of the path is selected, like below, it needs joining.

You may also get this message if you click the "calculate" button at the bottom of the toolpaths menu. This indicates you need to join paths.

You do this using the Join function. Select one path, press shift, click the 2nd path and click the join button. If you make a mistake, you can undo.

Next "add tabs" by ticking the tabs box

The defaults above are probably fine for the example, these just allow the piece to remain in place whilst you continue to cut, otherwise it may fall and hit the cutter and have a catastrophic failure.

Click "edit tabs"

For large objects (such as this chair) 2 is probably too few. You can select "constant distance between tabs" or specific a specific number, and whether you want to avoid corners and curved regions.

Too many means you have more cleanup, not enough risks the object falling, so pick appropriately and err on more than less for your own safety. We will select 4 for this object and click "Add Tabs".

The yellow T's show where the tabs are. You can drag and drop them only when on the tabs menu.

The above shows the cursor that appears when you hover over the tab.