A Guide to CNC Cover Gasketing: Improve Vacuum Hold-Down Performance

CNC Cover Gasketing Overview

Cover gasketing provides a reliable solution for securely holding small or irregular parts during CNC machining, especially when a standard MDF spoilboard cannot maintain sufficient suction. By creating a dedicated non-porous fixture with properly applied gasketing, the vacuum chamber seals more effectively, ensuring consistent hold-down, improved repeatability, and higher throughput. While the fixture requires additional setup time, it quickly pays off when producing multiple or high-volume parts.

Fixture Benefits

Provides strong, consistent hold for repetitive small-part cutting.
Enables reusing the same fixture for future production runs.
Reduces need for tabs or onion skins.

Instructions for Creating a Cover-Sheet Gasketing Fixture

1. Prepare the Fixture File

Import your file into VCarve or other software.
Generate the necessary Vectric toolpaths for cutting the small parts.

2. Build the Fixture

Construct the fixture from a non-porous material such as Baltic Birch, HDPE, or any other non-porous material such as Melamine, PVC, Corian, Phenolic to prevent vacuum loss.

Recommended Fixture Thickness:

3/4" (19 mm) material is the most commonly used and provides the best balance of rigidity, screw-holding strength, and durability.
1/2" (12 mm) material can be used for smaller parts or when weight is a concern, but it is more prone to flexing and can reduce vacuum performance.
Most Common: ¾” Baltic Birch or 3/4” HDPE, strong, stable and hold vacuum channels well with risk of warping.

Cut the cover gasket to match the full width of the fixture.

3. Select the Engraving Bit

A 30° engraving bit is recommended for cutting gasket channels.

4. Selecting the Right Gasketing Thickness

1/32" Thickness – Best for plastics or very smooth, consistent materials
1/16" Thickness - Common for wood applications with minor variation
1/8" Thickness – For warped or uneven materials requiring more compliance

5. Apply the Gasketing Material

Keep paper backing on during initial placement to prevent stretching while rolling it out.
Align the gasket, press it firmly to flatten it, and remove air pockets.
For stubborn air pockets, use a small pinhole to release trapped air.
Once positioned, remove the paper backing.

6. Cutting the Gasket Channels

Set the engraving bit depth to match the gasket thickness. Cut to the fixture surface but not through it.
Cut both the inner-diameter (ID) and outer-diameter (OD) channels that define the vacuum zones.
Oversize the channels slightly so the cutting tools do not contact or rub the gasket.
Ideally, the gasket should be placed as close to the toolpath as possible; while many users cut both the part and gasket in one pass with a standard end mill, using an engraving bit provides a cleaner gasket edge, so when cutting with a ¼" compression bit, the inner and outer toolpaths should be spaced about 0.25"–0.27" apart to accommodate the engraving bit.
We recommend a minimum gasket wall thickness of 1/8", which is the space between the toolpath and the inner vacuum pocket, though this may vary depending on part size and available vacuum area.

Recommended Spacing:

1/16” – 1/8” (1.5mm – 3mm) from part perimeter
For very small or easily shifting parts: as close as 1/16”
For larger parts with more surface area: 1/8” is ideal

A feed rate of 25 inches per minute at 18,000 RPM typically produces clean edges.
Periodically clean adhesive buildup from the engraving bit to maintain cut quality.

7. Finalize the Gasket Layout

Remove gasket material from the ID and OD channel areas to expose the toolpath region.
Ensure the channel width is larger than the tool diameter, so the gasket remains untouched during cutting.

8. Create Vacuum Pockets

Add internal vacuum pockets that feed suction to each part.
- For creating the vacuum pocket, you can either use an end mill to hollow out the cavity or route the inner and then outer perimeter with an engraving bit, ensuring both paths account for the gasket wall thickness.
Use one vacuum hole per part (recommended size: 1/4" or 3/8" diameter).
Add more holes when the part is large, long, has high surface area, multiple narrow sections, if the part tends to bow or warp or has uneven thickness or low rigidity.
Unused holes can be plugged as needed to maximize efficiency.
Scrap pieces can be used to cover unused vacuum holes when cutting additional parts.
Retain offcuts during machining or design vacuum zones to hold them until removal.
Blow off dust thoroughly before use.