Putting Datums and Geometric Tolerances on a Weldment That Moves
Geometric tolerancing on a machined part is well understood. Apply it to a part that was welded first and a set of new problems appears, because half the surfaces on the drawing were never cut by a machine and never will be.
Two tolerance systems on one drawing
The single most useful thing you can do on a weldment drawing is separate the two.
The welded structure is held to a general tolerance standard for fabrications. ISO 13920 is the common one. It gives tolerance classes A to D for linear and angular dimensions, and classes E to H for straightness, flatness and parallelism, scaled by the size of the feature. Class B with class F is a reasonable default for machine frames.
The machined features are held to a normal drawing tolerance, from ISO 2768 or ISO 286 for fits, or called out directly on the feature.
Put both on the drawing and say which applies where. A single general tolerance across a welded and machined part either prices the impossible or gets ignored, and both outcomes end badly.
Choosing datums that exist
A datum is a reference the inspector and the machinist both have to be able to find. On a weldment that rules out a lot of candidates.
Put the primary datum on a face that will be machined. It is the only surface you can trust to be where the drawing says.
Make sure a fixture can sit on it. A datum on the underside of a frame that has to be machined in the same setup as the features referenced to it is a contradiction. Somebody has to solve it and it is cheaper if you do.
Keep the datum features far apart. Three points close together on a 3 m frame amplify every small error into a large angular one. Spread them.
Do not over-constrain. A datum reference frame needs enough to lock six degrees of freedom and no more. Extra datums on a part that flexes create an impossible inspection.
A practical pattern for a machine base: primary datum is the large machined top or bottom face, secondary and tertiary are machined pads or a machined edge, and every bore and bolt pattern is positioned from that frame.
The controls that earn their place
Flatness on a machined mounting face. State the condition, for example flat within 0.1 mm after stress relief and finish machining. Without the condition it is unclear whether it is checked before or after the part relaxes.
Parallelism between two machined faces, or between a face and a datum. Common on rails and on frames that have to sit level.
Position on bores and bolt patterns. This is where GD&T pays for itself on a weldment, because position with a material condition modifier gives the shop the bonus tolerance it needs when the hole is at its most forgiving size.
Perpendicularity on a column or an upright relative to the base datum. Usually the tolerance that actually matters on a gantry.
Coaxiality or position on a line of bores. On a frame carrying a shaft through several bores, how well those bores line up is the whole job. Say it explicitly rather than hoping a positional tolerance from a distant datum covers it.
What to avoid
Machining tolerances on welded dimensions. The overall length of a welded frame is a fabrication dimension. Putting ±0.1 mm on it either forces the shop to machine both ends of a 3 m part or gets silently ignored.
Profile everywhere. It is the most general control and the most expensive to verify on a large part. Use it where the form matters and simpler controls where they do not.
Datums on surfaces nobody can reach. If the inspector needs to get a CMM probe or a height gauge to the datum face with the part in a stable position, check that it is possible on a 2 tonne frame.
Tolerance stacks that assume a rigid part. A large weldment sags under its own weight. A flatness callout measured with the part supported differently from how it is used gives a different answer. If the support condition matters, put it on the drawing.
How it gets inspected
On a large machined weldment the realistic methods are a portable CMM arm, a laser tracker, or a straight edge and feeler gauges for simple flatness. Each has a different uncertainty, and on a tolerance of a few hundredths of a millimetre across metres, the measurement uncertainty is a real part of the budget.
Ask in the RFQ what method the shop will use and ask for the report against the drawing revision. A dimensional report that references a superseded revision is a common and avoidable argument.
A short checklist
- Welded and machined tolerances are separate and both named.
- Primary datum is a machined face a fixture can sit on.
- Every geometric tolerance states the condition it applies to.
- Bores that must line up have an explicit control.
- The support condition is stated where the part will sag.
- The inspection method and the report requirement are in the RFQ.
Get those six right and the difference between quotes stops being a guess about what you meant.
Send your drawing and we will match it with shops that can hold it and prove it.
Frequently asked questions
Can a datum be on an as-welded surface?
It can, and it usually should not be. An as-welded surface moves with the distortion, so every feature referenced to it moves too. Put primary datums on faces that will be machined and that a fixture can physically sit on.
What is ISO 13920 and when does it apply?
It is a general tolerance standard for welded constructions. It gives classes A to D for linear and angular dimensions and E to H for straightness, flatness and parallelism. It applies to the welded structure, not to the features you machine afterwards.
Should I use profile of a surface on a weldment?
Sparingly. Profile is powerful and it is expensive to inspect on a large fabricated part. Use it where the form genuinely matters, and use simpler controls such as flatness and position where they do the job.
Need a quote for this part?
Send the drawing. We match you with up to 3 shops that weld and machine it in house, and we reply within 24 business hours.
Get matched with a weldment shop