Find where the tab first touches
If the corners contact while the flat sides have room, the internal cutter radius is a likely cause. An ideal 6.35 mm end mill leaves a 3.175 mm internal radius in an ordinary compensated rectangular slot.
If a straight face binds over most of its length, first measure the opening and tab. An undersized slot, oversized tab, wrong material thickness or a finish layer will not be corrected by simply increasing corner relief.
If the tab stops at the bottom, check slot depth, tab length and remaining chips before changing its outline. Relieve the corners, round the mating tab deliberately, or hand-finish them only after identifying the contact.
Fit clearance is not the dogbone bulge
Suppose a slot is 20.00 mm wide and its mating tab is 19.80 mm wide. The total width difference is 0.20 mm, giving 0.10 mm on each side when centred. That is a worked arithmetic example, not a recommended tolerance for every joint.
Even this clearance can leave square tab corners interfering with a slot cut by a 6.35 mm tool. Minimal relief on the 20 × 40 mm slot adds about 0.930 mm beyond each relieved wall, but the nominal straight-wall spacing remains 20 × 40 mm.
Choose assembly clearance for the actual material, finish, moisture, glue and desired fit. Measure stock thickness rather than relying on its nominal label. Set the intended slot size before adding relief; do not uniformly scale the relieved file to create clearance, because that also changes cutter-sized arcs.
Check the cutter used in CAM and on the machine
A 6 mm cutter is not a 1/4-inch cutter: 1/4 inch is 6.35 mm. The generator, CAM tool definition and cutter installed in the machine should agree.
For an ideal compensated inside profile, programming a 6.35 mm cutter while actually cutting with a 6.00 mm cutter can leave the opening 0.35 mm narrower. Runout, deflection and machine calibration can change the real result; measure a coupon rather than treating that calculation as a machining guarantee.
Use the finished contour for a pocket or a compensated inside operation as appropriate. A centreline operation or an extra manual cutter-radius offset changes the intended boundary.
Separate unit errors from machining errors
A factor near 25.4 points to an inch/mm conversion problem. SVG files from this generator carry physical millimetre dimensions; DXF R12 coordinates are millimetres even though the file is unitless. Check the imported outer extent against the generator before cutting.
If software dimensions are correct but the machined opening is wrong, investigate the cutter, compensation and machine. If the imported dimensions are already wrong, fix the import first. Relief is not a substitute for either check.
Use a small fit test before the final joint
Try the 20 × 40 mm, 6.35 mm minimal-relief example on this page. It is finished pocket geometry, not a matching tab generator. Adjust its nominal width and height to your measured stock and chosen clearance.
Export SVG or DXF, confirm the relief-inclusive dimensions in CAM, choose the same cutter, inspect the operation in simulation and test-cut scrap using suitable workholding. Measure the flat-wall opening and try the actual mating tab.
Record the cutter, stock thickness, programmed slot size, measured opening and first contact location. Change one cause at a time. A successful corner-relief preview does not certify machine accuracy, a universal press fit or a particular CAM version.