Every casting is made in a mould that has to open. Where it opens is the parting line, and it is usually the first real decision in casting design. It sets which way the draft runs, how many cores you need, where the flash ends up, and which dimensions get looser tolerances.
Last week we covered draft angle in casting, and the first rule there was to settle the parting line before adding a single degree of draft. This post covers that step: what a parting line is, the main types, how to choose one, and what it does to your tolerances, with a worked example you can follow.
The parting line is the line on a casting where the two halves of the mould met. The mating faces of the two halves are called the parting surface. The thin seam, or witness line, those faces leave on the finished part is the parting line.
The names change with the process, but the idea stays the same:
A parting line looks like a thin seam on a drawing. In practice it drives most of what happens next:
Most castings use one of four types.
| Type | What it looks like | When it is used | Watch out for |
|---|---|---|---|
| Straight (flat) | One flat plane through the part | Most parts, whenever the shape allows it | Nothing major; this is the default to aim for |
| Stepped (offset) | Two or more flat levels joined by a step | Parts with features at different heights | Costlier patterns, fins at the steps, more risk of swell in sand |
| Curved (contoured) | Follows the curve of the part | Curved housings, levers, crankshaft-like parts | Harder to make and fit, harder to keep flash tight |
| Split with side cores or slides | A main parting line plus extra moving parts | Side holes, pockets and undercuts that cannot come out straight | Every extra joint adds its own flash line and tolerance |
The industry rule of thumb is simple. A straight parting line is almost always the best choice, and it is often worth changing the part slightly to get one.
Work through these in order. Not every rule can win on every part, so the job is to find the best balance and agree it with the foundry or die caster early.
Take a simple sand-cast hub: a flange 120 mm in diameter and 15 mm thick, with a hub 60 mm in diameter rising 70 mm above it and a 30 mm bore through the middle. The hub has to run true to the flange. Here are three ways to split it.
| Option | How it is split | What works | What hurts |
|---|---|---|---|
| A: axis vertical, parting at the flange’s top face | Flange in the drag, hub in the cope | Straight line at the largest section; flange faces need no draft | Hub-to-flange alignment now crosses the parting line, so any shift shows as a step at the hub root |
| B: axis vertical, parting at the top of the hub | Whole casting in the drag | Straight line; flange and hub sit in one half, so they cannot shift against each other | A deep drag cavity (85 mm) with draft along the full height of the hub |
| C: axis horizontal, parting through the centre line | Each half holds half of every diameter | The bore core sits neatly in core prints in both halves | Every round surface crosses the parting line, and the flange faces now run along the draw, so they need draft |
If the hub-to-flange alignment is the critical requirement, Option B usually wins. Option A becomes the better choice when the hub is tall enough that the deep drag cavity gets awkward to mould. Option C is rarely the best answer for this part. The point is not the answer itself. It is that each option trades off draft, cores, mismatch and tolerance in a different way, and you should see those trade-offs before you model the details.
This is the part most students never hear about. When two mould or die halves close, they never meet perfectly. There is always a little gap, a little shift, or both. So a dimension that runs from one half to the other picks up extra variation that a dimension inside one half does not.
The North American Die Casting Association (NADCA) handles this with a simple rule. For any dimension across the parting line:
T_{total} = T_{linear} + T_{parting\ line}The parting line tolerance is plus only, because the halves can be held slightly apart but never pushed closer than fully closed. It grows with the projected area of the casting, which is the area you see when you look at the part straight down the direction the die opens.
| Projected area | Aluminium | Zinc | Magnesium |
|---|---|---|---|
| Up to 64.5 cm² (10 in²) | +0.14 mm | +0.114 mm | +0.14 mm |
| 71 to 129 cm² (11 to 20 in²) | +0.165 mm | +0.13 mm | +0.165 mm |
| 135.5 to 322.6 cm² (21 to 50 in²) | +0.19 mm | +0.15 mm | +0.19 mm |
| 329 to 645.2 cm² (51 to 100 in²) | +0.30 mm | +0.23 mm | +0.30 mm |
| 651.6 to 1290.3 cm² (101 to 200 in²) | +0.46 mm | +0.30 mm | +0.46 mm |
| 1296.8 to 1935.5 cm² (201 to 300 in²) | +0.61 mm | +0.46 mm | +0.61 mm |
These are NADCA standard values, added to the linear tolerance. For larger parts, NADCA says to consult your die caster. Slides and moving cores follow a similar idea, with their own plus-only tolerance.
An aluminium die-cast housing has a projected area of about 100 cm². You need to hold a 76.2 mm (3 in) height.
NADCA’s standard linear tolerance for aluminium is ±0.25 mm for the first 25.4 mm, plus ±0.025 mm for each additional 25.4 mm. For 76.2 mm that is ±0.25 + 2 × 0.025 = ±0.30 mm.
Same part, same machine, but 0.165 mm extra on one side simply because of where the die splits. If that height is critical, move it into one half or plan to machine it.
Sand moulds are less rigid than steel dies, so shift is a bigger factor. One common design guide suggests planning for parting line mismatch of up to about 0.5 mm (0.020 in), and seam flash of up to about 0.4 mm (0.015 in). Treat these as planning figures, not a standard. Real values depend on the foundry, the moulding method and the part size. ISO 8062-3 treats surface mismatch separately from the general dimensional tolerances, so ask your foundry which tolerance grade they quote and how they handle mismatch.
These show up again and again in the casting projects we review during training:
Run through this before you add draft or detailed features:
Because the two halves never close perfectly. NADCA adds a plus-only parting line tolerance, from +0.114 mm upwards depending on alloy and projected area, to any die-cast dimension that crosses the joint.
Mismatch, or shift, is when one half of the mould moves slightly against the other. It shows up as a small step on the casting at the parting line.
The idea is the same: the line where the tool halves meet. The numbers differ, because metal shrinks differently and sand moulds behave nothing like steel injection tools. Our plastic component design guide covers the plastic side.
A parting line is easy to draw and hard to choose well. That judgement comes from seeing real castings, real patterns and real rejections, not from CAD commands alone.
Navinyasa’s Casting Component Design Training in Bengaluru covers casting materials, sand, die, gravity and investment casting, tool direction, parting line identification and draft, with live projects and mentor guidance. Book a free demo or WhatsApp us at +91 990 113 6476.
