A board can look perfect on screen and still be wrong by half a millimetre. Visual inspection catches the dramatic export failures — mirrored layers, missing files, holes beside pads — but the failures that scrap boards quietly are numerical: a connector footprint whose pads are a pitch too narrow, a mounting hole that moved, a clearance that shrank below what the board house can etch. Gerbv’s answer is measurement on the displayed image, a core part of the viewer since its early releases: you measure the exported data itself, not the design intent in your EDA tool, so what you read is what the factory will work from. This tutorial covers the measurement workflow, how to read coordinates and distances sensibly, and the specific checks — trace and space, hole sizes, board dimensions — that are worth doing before every order. Install Gerbv first with the Windows installation guide or your platform’s guide from the download page, and see our Gerber viewer page for where measurement sits in the overall inspection.
The measurement workflow
Open the board and stack the layers you need, following loading and aligning Gerber layers so the geometry is in registration. Zoom in until the feature you want to measure fills a good part of the window — measurement precision in any viewer is limited by how precisely you can place the measurement points, and at full magnification a pad edge is a clear target instead of a guess. Then use the measure tool on the displayed image: mark the two points that define the distance — opposite edges of a pad, centres of two holes, the two sides of a gap — and read the result. Measure each critical feature twice, approaching it fresh the second time; if the two readings disagree, your point placement, not the board, is the noise, and zooming further usually settles it. Work from a short written list of the dimensions your design actually depends on rather than measuring at random: the goal is verifying specific intended values, not admiring numbers.
Reading coordinates, not just distances
Distances tell you sizes; coordinates tell you positions, and positions are where export surprises hide. Note the coordinates of a known reference — a mounting hole centre or a corner of the board outline — and compare them with the mechanical drawing or the enclosure the board must fit. Then check a second reference at the opposite side of the board. If both positions are right, the board’s overall scale is right; if the first is right and the second is off by a growing margin, suspect a unit problem in the export, because a millimetre file read as inches (or the reverse) produces exactly that signature. Gerbv’s documented export options work in inch, millimetre and mil units, which is a reminder of how central units are to this data: Gerber files carry their unit and coordinate format in the file, and a mismatch between what the EDA tool wrote and what anyone assumes is a classic source of boards that arrive the wrong size. Coordinates also settle alignment arguments: two features that should share an axis should share a coordinate, exactly, in the data.
The checks that matter: trace/space, pads and holes
Three families of measurement repay the effort on every board. Trace and space: measure the width of the thinnest traces and the gap between the closest pair, especially where routing passes between pads. Those two numbers are your manufacturing margin — they should sit comfortably inside the capability of the board house you will use, with room for the fact that etching is a physical process, not an ideal one. Pads and annular rings: measure a few representative pads, and for plated holes, compare the pad diameter with the drill diameter from the drill layer — the difference, halved, is the annular ring the drill has to land in, and a ring that is thin on screen will be thinner, or broken, after real drill wander. Holes themselves: measure drill hits against the sizes your components need — connector pins, mounting hardware, press-fit parts — remembering that a finished plated hole ends up smaller than the drill that made it. Gerbv’s report windows support this pass: they summarise the Gerber and drill codes used in the files, and the aperture-usage reporting shows how often each aperture is used across the visible layers, which helps you confirm that the set of sizes present is the set you expected.
Board-level dimensions and the 1:1 sanity check
Finish at board level. Measure the outline’s overall width and height and at least one diagonal, and the distances from a mounting hole to two board edges. These are the numbers an enclosure, a panel or a mating connector will judge the board by, and they are the fastest possible detector of a scaled export: if the outline measures ten times or 2.54 times the intended size, units went wrong somewhere and nothing else in the set can be trusted until that is fixed. The same known dimension becomes your reference if you go on to print the board at 1:1 scale for a paper fit check — print, measure the same feature on paper, and the print is verified. And keep the limit of all this in view: Gerbv measures what you point at. It does not scan the board against a rule set — there is no DRC or DFM checking in Gerbv — so a measured pass on your checklist plus the board house’s own checks is the safety net, not either one alone.
Recording what you measured
Measurements you cannot show anyone are half wasted. Note the intended value, the measured value and the layer for each item on your checklist, and consider exporting the relevant view — Gerbv exports PNG, PDF, PS, SVG and DXF, covered in exporting to PDF, PNG or SVG — with the record. When a board comes back wrong, that record is what turns an argument about whose fault it is into a lookup: either the exported data measured wrong before ordering, or the data was right and manufacturing drifted. Both answers are useful; not knowing is not.
Frequently asked questions
What should I measure first in Gerbv?
Start with the board outline’s overall size and one mounting-hole position — they catch scale and unit errors instantly. Then measure the thinnest trace and tightest gap, representative pads, and the drill sizes your components depend on.
Can Gerbv check my clearances automatically?
No. Gerbv measures the distances you point at and reports statistics about the codes used, but it has no design-rule or DFM checking. Automatic rule checking remains your EDA tool’s and your board house’s job; measurement is how you verify the exported result.
My measured size is off by a factor of about 2.54 or 10. What happened?
That signature points at a unit or coordinate-format mismatch in the export — millimetres read as inches differ by 25.4, and format precision errors commonly show as factors of ten. Re-check the export settings in your EDA tool and re-export the full set.