How to Auto Bridge on CypCut CNC Machine

• 1
  Key takeaways
• 2
  What auto bridging does on a CypCut CNC machine
• 3
  When auto bridge on CypCut is worth using, and when it is not
• 4
  Tab width, tab count and spacing that hold up in production
• 5
  Where to place tabs so they do not damage the part
• 6
  Three failures that show up after auto bridging
• 7
  Step by step: how to auto bridge on CypCut
• 8
  Tab width and count by material and thickness

A fiber laser cuts a closed contour and the part falls. Sometimes it does not fall cleanly. It tips, catches the nozzle, or slides under the slats and gets scratched by the next sheet. Auto bridging solves that by leaving one or more short uncut segments along the contour. The part stays connected to the sheet skeleton until an operator breaks the tabs by hand or with a small chisel.

In CypCut, bridging lives in the cutting layer parameters, not in the nesting module. You set a tab count and a tab width for the layer, and the software inserts the uncut segments when it generates the tool path. Because it is a layer setting, a 1 mm stainless layer and a 3 mm mild steel layer can use different tab values on the same nest.

The feature is often confused with micro-joints in other CAM packages. The idea is the same. The difference is where you control it: CypCut exposes tab width, tab count and the tab placement mode directly in the layer dialog, so you can tune per material without rebuilding the nest.

Auto bridging does not change the part geometry. The contour is still cut to the drawing. The tab is a handling aid that you remove downstream. If a part has a cosmetic edge or a sealing face, put the tabs on a non-critical edge instead of disabling the feature.

Use it when the part is small relative to the sheet, when it has a high length-to-width ratio, or when the contour is a full closed loop with no natural connection to the skeleton. Long thin brackets, gaskets and shim plates are the classic cases. Without tabs, these parts rotate on the slats and the next rapid move drags them into the nozzle.

Use it when the material is thin. Sheet below 1.5 mm has little stiffness, and even a part with a reasonable footprint can lift at the corners as the cut releases residual stress. Two or three tabs keep the part flat until you lift the whole sheet.

Skip it when the part is heavy and stable. A 6 mm plate with a compact outline will not move. Adding tabs there only costs you a deburring step. Skip it too on parts where the entire contour is a functional sealing surface, unless you can place the tab on a corner that gets machined later.

One more limit: auto bridging works on contours, not on internal cutouts you intend to drop out. If a slug inside the part must fall free, keep it tab-free and let it drop into the collection tray. Bridging the slug creates a loose piece you have to fish out by hand.

Tab width is the length of the uncut segment along the contour. The metal left there is a small bridge, and its strength scales with width and with sheet thickness. On 1 mm mild steel, 0.6–0.8 mm is enough. On 3 mm mild steel, 1.0–1.5 mm is comfortable. Above 6 mm sheet, tabs get expensive to break, so consider whether you need them at all.

Tab count depends on the perimeter. A rough rule: one tab for every 80–120 mm of contour length, with a minimum of two per part. Two tabs on opposite sides stop rotation. Three tabs spaced at roughly 120° are better for round parts because they stop both rotation and lift.

Spacing matters more than count on long parts. If you put all tabs on one end, the free end can still flap. Distribute them evenly. Most CypCut versions offer an evenly spaced mode; use it unless you have a specific edge that must stay tab-free.

For stainless and aluminum, reduce tab width by about 20 percent compared with mild steel of the same thickness. Both materials work-harden at the tab, and a wide tab on 304 stainless can tear a notch into the edge when you break it off. On aluminum, a wide tab also bends the part before it snaps.

Put tabs on straight edges when you can. A tab on a straight run breaks cleanly with a light bend. A tab on a tight radius concentrates stress and can pull material from the arc, leaving a visible dent. If the part is all curves, place tabs at the tangent points between arcs, not at the apex of a small radius.

Keep tabs away from the lead-in. The pierce point and lead-in carry spatter and a small amount of dross. If a tab sits right next to the lead-in, that dross fuses to the tab and you have to grind it off. Offset the tab by at least 5–10 mm from the lead-in end.

On parts with a machined face, place tabs on the side that gets the least finishing. For a bracket that will be anodized, a tab mark on an edge is usually acceptable because the anodize line hides it. For a sealing face or a bearing bore edge, move the tab to an outer profile or add a machining allowance.

Finally, check tab placement against the slat positions. A tab that sits directly over a slat gap is harder to support when you break it. Not a hard rule, but it saves a dropped part on a busy shift.

The part tips even with tabs. This usually means the tabs are too narrow for the part mass, or they are clustered on one side. Check the preview for placement first, then widen by 0.2 mm. On parts over 200 mm long, add a third tab in the middle before you touch the width.

The tab tears the edge when broken. The tab is too wide or the material is work-hardened. Reduce width by 20 percent and move the tab to a straight edge. On 304 stainless, add a small relief notch at each end of the tab in the drawing if the edge is visible after assembly.

The part shifts during cutting, before the contour closes. This is not a bridging problem. It means the skeleton itself is moving because inner cuts released stress. Cut a stress-relief pass or reorder so inner features go last on that part, and check the sheet is flat on the slats.