Datums, Flatness and Squareness on a Machine Base Drawing

How to choose datums for a large weldment or casting, which geometric controls belong on a machine base, and the drawing habits that cause inspection disputes.

Most inspection disputes on machine bases are not measurement problems. They are drawing problems, and specifically datum problems: two competent people measured the same part correctly against different references and got different answers.

Why the datum is the whole game

A tolerance without a datum is often meaningless. Flatness is the exception, because it constrains a surface to itself. Everything else on a machine base, parallelism, squareness, perpendicularity, position, is a relationship, and a relationship needs something to relate to.

If the drawing does not say which surface is the reference, the inspector picks one. Probably a sensible one, probably not the same one your designer had in mind, and probably not the one the machine actually sits on.

Choosing datums that match how the machine works

The primary datum should be the surface the machine’s accuracy actually hangs from. On most bases that is the main mounting face: the plane that carries the rails, the ways or the table.

Then:

• Primary constrains three degrees of freedom. Usually the largest functional plane.
• Secondary constrains two more. Often an edge, a machined side face, or a pair of dowel holes.
• Tertiary constrains the last one.

Two practical tests for a proposed datum scheme:

1. Can it be physically realised? The inspector has to set the part on that primary datum. If the primary is a surface facing downward in the only stable orientation, the scheme is a problem.
2. Does it match assembly? If the base is assembled against face A but toleranced from face B, your tolerance stack does not describe the machine you are building.

That second one is worth pausing on. It is common to see a base dimensioned from a convenient edge while the machine is actually located by dowels in a pad. Every tolerance on that drawing is then describing a relationship nobody cares about.

Which controls belong on a machine base

Flatness on each functional pad, and separately on the overall mounting plane if that matters. Remember these are different requirements: individual pads can each be flat while not being coplanar with each other.

Parallelism where two faces must stay in a fixed relationship, such as rail pads relative to the mounting plane. This is usually what people mean when they write flatness on a second face.

Perpendicularity for a column mounting face relative to the bed, or a bore axis to a face. Frequently the tightest real requirement on the part and frequently omitted.

Position for dowel and bolt holes, ideally with the material condition modifier your standard supports, which gives back tolerance when features are away from their worst condition and costs you nothing in function.

Profile for anything curved or compound, where it does the work of several controls at once.

Coplanarity, expressed as a profile control across multiple pads, for the common case of several mounting pads that must together form one plane. This is the requirement people most often try to express with flatness on each pad and then find does not say what they meant.

Drawing habits that prevent arguments

Reference the standard. State ISO 1101 or ASME Y14.5 and the year, once, in the title block. A drawing that mixes conventions gets interpreted twice.

Do not tolerance everything. A default tolerance note covers non-functional geometry. Geometric controls go on functional features only. A drawing with a control frame on every face tells the shop nothing about what matters, and they will price the tightest number on the page across the whole part.

State the fabrication tolerance class separately. The weldment before machining is covered by ISO 13920 class A to D. That is a different requirement from the machined geometry and needs saying explicitly, or the fabricator will assume the loosest class that is defensible.

Define the inspection condition. Support scheme, temperature, and whether the part is free-standing or bolted down. On a large structure this changes the measured result more than any instrument choice: see measuring flatness.

Say what is inspected and what is reported. Not every controlled feature needs a number in the report. Mark which are pass or fail, which are recorded for information, and which are first-article only.

Provide datum targets on rough surfaces. If something must be checked before machining, use datum targets: specific points, lines or areas rather than a whole distorted surface. It is the correct tool for exactly this problem and it is rarely used.

A minimum viable scheme

For a straightforward machine base:

• Datum A: main mounting plane, flatness controlled.
• Datum B: a machined side face or a dowel pair, perpendicular to A.
• Datum C: the remaining orthogonal reference.
• Coplanarity across the mounting pads as a profile control to A.
• Parallelism of rail pads to A.
• Perpendicularity of the column face to A and B.
• Position on dowels relative to A, B and C.
• A general fabrication class for everything else.

Eight lines. They cover the great majority of bases and they can be inspected by anyone, anywhere, with the same result.

Common questions

← All guides