How Much Stock to Leave on a Weldment Before You Machine It
Welding moves metal. Every joint shrinks as it cools, and a frame that was flat on the fit-up table is not flat when it comes off. That is normal and it is designed around, not prevented. The part you machine is never exactly the part you drew, and the drawing has to say which condition each number applies to.
Start with the allowance
Machining allowance is the extra material left on a face so that the cutter can clean it up after everything has moved.
Leave too little and the face cleans up in one corner and still shows weld spatter and mill scale in the other. Leave too much and you have doubled the machining time and possibly cut through into a weld you needed.
As a starting point:
| Feature | Typical allowance |
|---|---|
| Machined face on a short, stiff part | 3 mm |
| Machined face on a long or lightly braced part | 5 to 6 mm, sometimes more |
| Bore to be line bored | About 3 mm on the radius |
| Face that will be ground after machining | Add 0.3 to 0.5 mm on top |
These are starting points, not rules. The real number depends on the length of the part, the amount of weld metal, how restrained the joints are and whether the part will be stress relieved. A good shop will tell you it wants more on one face and less on another, and that answer is worth more than the table.
Split the tolerances
Put two tolerance systems on the drawing and say which applies where.
The welded structure is normally held to a general tolerance standard for welded constructions. ISO 13920 gives classes A to D for linear and angular dimensions and classes E to H for straightness, flatness and parallelism. Class B and class F is a common, sensible pairing for machine frames.
The machined features then carry a normal drawing tolerance, from a general standard such as ISO 2768 or directly on the feature.
Writing one tight general tolerance across the whole drawing is the fastest way to a quote full of assumptions, because the shop has to either price the impossible or guess at what you meant.
Put the datums where a machine can reach them
Pick datum faces that will be machined and that a fixture can sit on. Three practical checks:
- Can the part rest on the datum face without rocking, or does it need packing that will itself become an error?
- Is the datum reachable once the part is in the machine, or does the spindle have to travel through the workpiece to touch it?
- Does the datum face get machined in the same setup as the features referenced to it? If not, you have introduced a second setup into the tolerance chain.
Say when each number applies
A machine base drawing that says “flatness 0.05 mm” without a condition invites two different quotes. Flatness on a machined face is achieved after machining, and it holds only if the part was stress relieved first. Write the condition on the drawing, for example “after stress relief and finish machining”, so the part is inspected the same way it was quoted.
The same applies to bore alignment. Bores line bored in one setup after stress relief are a different job from bores bored before stress relief, and the second one is not a job at all.
Sequence in short
For most machined weldments the sequence that works is: cut and prepare, fit and tack, weld to a planned sequence, inspect the welds, stress relieve, rough machine if there is a lot of stock, finish machine, then coat with the machined faces masked.
Moving stress relief after machining, or moving galvanising after machining, are the two changes that most often show up as a part that measured correct at the shop and wrong on your floor.
What to check before you send the drawing
- Machining allowance is stated, not assumed.
- The weldment tolerance and the machining tolerance are separate and both named.
- Datums are on faces that will be machined.
- Every geometric tolerance says which condition it applies to.
- The finish note says which faces are masked.
Five lines on a drawing, and they remove most of the questions a shop would otherwise price as risk.
Frequently asked questions
How much machining allowance should I leave on a weldment?
A common starting point is 3 to 6 mm on faces and about 3 mm on the radius of a bore, with more on long or thin sections that are likely to move. The right number depends on the part length, how much weld went in and whether it is stress relieved, so it is worth agreeing with the shop rather than copying a default.
Can I put one general tolerance on a weldment drawing?
Not usefully. The welded structure and the machined features need separate tolerances, because they are produced by different processes with different capability. ISO 13920 covers general tolerances for welded constructions and a normal drawing tolerance such as ISO 2768 covers the machined features.
Should the datum be on a welded face or a machined face?
On a machined face wherever you can. A datum on an as-welded surface moves with the distortion, and every feature referenced to it moves with it. Pick datum faces that will be machined and that a fixture can physically sit on.
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