How to mark critical dimensions for FDM production
How to flag the dimensions that actually matter on a drawing, use datums and general tolerance notes correctly, and avoid over-toleranced FDM drawings.
Drawings that arrive with every single dimension toleranced to plus or minus 0.05 mm slow down quoting and rarely reflect what the part actually needs. Drawings with no tolerance information at all put the burden on us to guess which features matter. Neither extreme helps you get a part that fits and costs what it should. The fix is straightforward: identify the small number of dimensions that are genuinely functional and mark only those clearly.
This guide covers how we like to see critical dimensions marked on an incoming drawing, what a sensible general tolerance note looks like for FDM, and how to set up a datum structure that actually means something for a printed part.
What actually counts as a critical dimension
A dimension is critical if it mates with another part, if it defines a clearance or interference that affects function, or if it drives an assembly stack-up across several components. Wall thickness for stiffness, general envelope size, and cosmetic proportions are almost never critical in this sense, they only need to sit within a sensible general tolerance band. If you cannot explain in one sentence why a dimension needs to be exact, it probably does not.
- Bore or shaft diameters that carry a bearing, bushing or pin
- Mounting hole patterns that must match an existing bracket or enclosure
- Slot widths or channel widths for sliding or telescoping parts
- Thread pitch diameters and insert bore diameters
- Any dimension that appears in more than one part of an assembly
Marking critical dimensions on the drawing
The clearest way to flag a critical dimension is a boxed tolerance value directly on that dimension line, combined with a note pointing to the mating part or assembly if that context is not obvious from the drawing alone. Colour highlighting or a simple revision cloud around the value also works well in a PDF review copy, even if it is not part of the formal drawing standard, because it tells us immediately where to focus during DFM review rather than making us cross-reference every dimension against the 3D model.
For everything else, a single general tolerance note covers the drawing. We typically recommend a note along the lines of ISO 2768-m adapted for FDM, stated once in the title block, so that anyone reading the drawing knows the default band without needing every dimension individually labelled.
| Nominal size range | Suggested general tolerance |
|---|---|
| up to 30 mm | +/- 0.15 mm |
| 30 to 100 mm | +/- 0.25 mm |
| 100 to 200 mm | +/- 0.4 mm |
| above 200 mm | +/- 0.2% of nominal |
Setting up a datum structure that means something
Even without full GD&T, a simple primary, secondary and tertiary datum reference on the drawing removes ambiguity about where a dimension is measured from. For a printed part, we recommend choosing datums that correspond to features you can actually locate reliably after printing, such as a flat base or a machined reference hole, rather than a theoretical centre point buried inside the part. If two parts must mate, both drawings should reference the same physical features as datums so both sides are measured consistently.
Over-tolerancing costs you money without adding value
When every dimension on a drawing carries a tight tolerance, we cannot tell during quoting which ones actually require secondary machining and which were toleranced out of habit from a CNC drawing template. The safe assumption then becomes that everything needs checking or reworking, which raises the quoted price and lead time for no functional benefit. We see this often on drawings converted directly from a machined part without adjusting the tolerance scheme for the new process.
- Problem
- All 14 dimensions toleranced at plus or minus 0.05 mm, inherited from the original milled part drawing.
- Change
- Reviewed with the customer, only 2 mounting hole positions were actually functional, the rest moved to a general FDM tolerance note.
- Result
- Quoted lead time dropped from 9 to 5 working days, no secondary machining needed except on the 2 flagged holes.
What we do if a drawing has no tolerance information at all
If a drawing or a 3D file arrives with no tolerance callouts, we do not simply guess. During the DFM review we identify the features that look functional from geometry alone, such as bores sized to a standard bearing or shaft diameter, and confirm with you which of these actually need a specific tolerance before we quote. This short back and forth upfront avoids a mismatch discovered only at first article inspection.
Frequently asked questions
- How many dimensions on a drawing should be individually toleranced?
- As few as possible, usually only the handful that mate with another part or drive an assembly stack-up. Everything else should fall under a single general tolerance note.
- What general tolerance should I use for FDM parts?
- A note similar to ISO 2768-m, adapted for FDM, works well as a starting point: roughly plus or minus 0.15 mm up to 30 mm, widening as the dimension increases. We can confirm the exact band for your material during quoting.
- What happens if my drawing has no tolerance information at all?
- We identify features that look functional from geometry, such as standard bearing bore sizes, and confirm with you which need a specific tolerance before quoting, rather than guessing or assuming everything is critical.
- Why does over-tolerancing increase my quoted price?
- If every dimension looks critical, we have to assume every dimension needs checking or secondary work, which adds inspection time and sometimes machining that the part does not actually need functionally.
- Do I need formal GD&T on my drawing for FDM parts?
- Not usually. A simple datum reference and clearly marked critical dimensions with a general tolerance note cover most FDM parts well. Full GD&T is worth the effort mainly for complex assemblies with tight stack-up requirements.
Have your part reviewed before production
Send us your CAD file together with the application, load and operating conditions. We review geometry, orientation, material and tolerances and come back with concrete change proposals and a quote.
Read next
FDM Tolerances and Fits: What Accuracy Is Realistic
A practical look at what dimensional accuracy you can actually expect from FDM parts and how to design tolerances and fits around it.
Clearance and Transition Fits for FDM Parts
A working reference for how much clearance to design into mating FDM parts, from loose running fits to interference press fits.
Designing Holes for FDM 3D Printing
A practical guide to why holes fail on FDM parts and how to design them so they print round, sized and functional.
Reducing Cost Through Design: The FDM Cost Guide
A practical breakdown of what drives FDM unit price and which design changes reduce it without cutting into part performance.
Post-Processing to Reach Tighter Tolerances on FDM Parts
A practical overview of secondary operations that bring specific FDM features to a tighter tolerance than the raw print delivers.