Least Material Condition (LMC) in GD&T

Introduction

A feature can be within its size tolerance and still create a problem if its location leaves too little material around it. This matters when a hole is close to an edge, when a slot leaves a thin section, or when a shaft must retain a minimum amount of material.

Least Material Condition (LMC) is used in GD&T when the design needs to control this type of condition.

For a hole, LMC is the largest allowed diameter because a larger hole leaves less material around the feature. For a shaft or pin, LMC is the smallest allowed diameter because a smaller shaft contains less material.

The practical reason for using LMC is not simply to allow a feature to vary more. It is to control the relationship between feature size, feature location, and the amount of material that must remain around the feature.

What Is Least Material Condition (LMC)?

Least material condition (LMC) in GD&T - Mechademic

Least Material Condition (LMC) is the size condition of a feature where the feature contains the least material allowed by the specified size limits.

In GD&T, LMC applies to a feature of size, such as a hole, shaft, pin, or similar feature. The LMC value comes directly from the feature's size limits on the drawing.

The term minimum material condition may appear in related GD&T discussions, but Least Material Condition (LMC) is the standard term used in GD&T.

LMC for Holes and Shafts

MMC and LMC for holes (ScienceDirect)

To find LMC, look at the two permitted sizes and determine which condition leaves less material in the feature.

For an internal feature, such as a hole, the larger diameter is LMC.

For an external feature, such as a shaft, the smaller diameter is LMC.

The useful rule when reading a drawing is: for a hole, look at the largest permitted diameter; for a shaft, look at the smallest permitted diameter.

LMC Symbol and GD&T Drawing Callouts

LMC callout (Machining Doctor)

The LMC modifier is shown by the circled L symbol Ⓛ in a feature control frame. It tells the reader that the geometric tolerance is related to the feature's least material condition.

For example:

Position | ⌀0.20 | Ⓛ | A | B

When reading this callout, do not look at ⌀0.20 by itself. Read the complete feature control frame together with the feature's size limits and the referenced datums.

The Ⓛ is placed directly after the geometric tolerance when the tolerance is controlled at LMC.

For example:

Position | ⌀0.20 Ⓛ | A | B

The engineering drawing reader should identify four things:

1. Geometric characteristic: here, position.
2. Stated geometric tolerance: ⌀0.20.
3. Material condition modifier: Ⓛ, meaning LMC.
4. Datum references: A and B, which establish the reference system for the geometric requirement.

The feature's size limits still come from the dimension callout. The LMC symbol does not replace or change those limits. Instead, it tells the inspector how the geometric tolerance is to be evaluated in relation to the feature's actual size.

MMC vs LMC vs RFS in GD&T

MMC, LMC, and RFS differ in how the geometric tolerance relates to the actual feature size.

For holes, MMC is the smallest permitted diameter, and LMC is the largest. For shafts and pins, the direction is reversed: MMC is the largest permitted diameter, and LMC is the smallest.

RFS does not select a particular size limit. The geometric tolerance is evaluated at the actual feature size without adding a material-condition allowance.

When LMC Is Used Instead of MMC

Least Material Condition (LMC) (GD&T Basics)

LMC makes sense when the problem is losing too much material, rather than having insufficient clearance for assembly.

A typical case is a hole located close to an outside edge. If the hole becomes larger or moves too close to the edge, the remaining wall becomes thinner. An LMC requirement can be used when that minimum wall condition needs to be controlled.

MMC is commonly selected when assembly or worst-case fit is the controlling function, while LMC is commonly selected when minimum remaining material is the controlling function.

So the choice depends on what the feature needs to protect:

• MMC: assembly clearance
• LMC: remaining material
• RFS: fixed geometric tolerance independent of feature size

For a detailed explanation of MMC and its effect on geometric tolerance, see our MMC in GD&T guide.

LMC, Bonus Tolerance, and Virtual Condition

An LMC modifier makes the actual feature size part of the geometric-tolerance calculation. The stated tolerance applies at LMC; when the feature moves away from LMC, the difference can be used as additional geometric tolerance.

LMC itself is a feature-size condition, not a virtual condition. When an LMC-controlled geometric tolerance combines with the LMC size limit to establish a boundary, that boundary is the virtual condition for the feature.

Bonus Tolerance at LMC

LMC modifier applied with a position tolerance (ResearchGate)

For an LMC-controlled feature, compare the actual measured size with the LMC limit.

• For a hole, a smaller actual diameter than LMC provides additional tolerance. Bonus tolerance = LMC size − actual size.
• For a shaft, a larger actual diameter than LMC provides additional tolerance. Bonus tolerance = actual size − LMC size.

This means the applicable geometric tolerance cannot be determined from the feature control frame alone. The actual feature size is also required to calculate the available bonus tolerance.

LMC Bonus Tolerance Calculation Example

Drawing using LMC Position Tolerance (ResearchGate)

A hole is specified as:

Ø10.00 +0.05 / −0.00 mm
Position | ⌀0.20 | Ⓛ

The LMC size is Ø10.05 mm.

During inspection, the hole measures Ø10.02 mm.

LMC departure: 10.05 − 10.02 = 0.03 mm

The available position tolerance is therefore: ⌀0.20 + ⌀0.03 = ⌀0.23 mm

The applicable position tolerance for the measured hole is therefore ⌀0.23 mm, including the ⌀0.03 mm of bonus tolerance.

Virtual Condition at LMC

Virtual Condition vs Tolerance Zone (GD&T Basics)

Virtual Condition is a boundary established by the applicable feature size and geometric tolerance when the geometric tolerance is modified by MMC or LMC. LMC itself is the feature-size condition used in that calculation.

For an internal feature such as a hole, the LMC virtual condition is calculated by adding the geometric tolerance to the LMC size:

Virtual Condition = LMC size + geometric tolerance

Using the example above:

• LMC = Ø10.05 mm
• Position tolerance at LMC = Ø0.20 mm
• Virtual Condition = Ø10.05 + Ø0.20 = Ø10.25 mm

For an external feature such as a shaft or pin, the calculation uses the opposite direction:

Virtual Condition = LMC size − geometric tolerance

The virtual condition should not be confused with the actual feature size or the bonus tolerance. LMC establishes the applicable size condition, bonus tolerance increases the available geometric tolerance as the actual feature departs from LMC, and the virtual condition represents the resulting boundary from the specified size and geometric tolerance.

Why LMC Matters in Part Design

LMC becomes useful when the feature itself can remove material from an already limited section of the part. The drawing then needs to control the feature in a way that protects the remaining section, rather than looking at the feature diameter or position separately.

Minimum Wall Thickness and Edge Distance

Take a Ø10 mm hole located 3 mm from the edge of a plate. The important dimension is not only the hole center location. The remaining material between the hole and the outside edge must also stay within the design requirement.

The same issue appears when:

• A hole is close to the end of a flange.
• Two holes are close enough that their edges approach each other.
• A drilled hole is close to a pocket, slot, or internal cavity.
• A counterbore removes additional material around an existing hole.
• A thin boss has a hole running through its center.

For these features, the designer needs to consider the actual material left after the feature is produced. LMC can be applied when the minimum-material condition is the functional concern.

Functional Requirements

The reason for using LMC should come from what the part has to retain.

For example, suppose a mounting hole is close to an outside edge. The design may require at least 2 mm of material between the hole boundary and the edge. A feature that is within its diameter tolerance can still create a problem if its location leaves less than the required material.

The same principle applies to a thin wall around a bore. If the wall must remain above a specified thickness for strength, sealing, or support, the drawing needs a geometric requirement that addresses the relationship between the bore and the surrounding geometry.

This is where LMC has a practical purpose: it connects the feature's size and location to the material that must remain in the finished part.

Limitations of LMC

LMC is not automatically the right modifier for every hole near an edge.

If the actual requirement is simply:

“Keep at least 2 mm of material between this hole and the edge.”

Then the drawing may need a direct edge-distance, profile, or location requirement, depending on how the feature is functionally controlled.

LMC is most useful when the designer specifically wants the feature's size and geometric tolerance to interact at the least-material condition.

It also requires a drawing that clearly establishes the feature size, geometric control, and applicable datums. Without those details, an LMC symbol by itself does not define the complete manufacturing requirement.

How LMC Affects CNC Machining and Inspection

With an LMC-controlled feature, the machinist and inspector need to look at feature size and geometric location together. The actual size of the finished feature determines how much geometric tolerance is available under the LMC callout.

CNC Machining Considerations for LMC Features

The machining process still has to keep the feature within its specified size limits. At the same time, the feature location must stay within the applicable geometric requirement.

For production work, this means watching for changes in feature size caused by:

• Tool wear
• Tool deflection
• Cutting-condition changes
• Tool-setting errors
• Part positioning errors

For example, if a hole is controlled at LMC, producing the hole at different sizes within its permitted range can change the geometric tolerance available to that hole. The CNC process therefore needs enough control over both hole size and location rather than treating the diameter as the only critical value.

Inspecting LMC-Controlled Features

Inspection should establish two values:

1. Actual feature size
2. Actual geometric deviation

The measured size is needed to determine the applicable geometric tolerance under the LMC callout.

For example, if a hole has an LMC size of Ø10.05 mm and a position tolerance of ⌀0.20 mm at LMC, a measured hole of Ø10.02 mm has a 0.03 mm departure from LMC. The available position tolerance is therefore ⌀0.23 mm.

For a CMM inspection, the actual feature size is first established from the measured feature, and the applicable position tolerance is then determined from the LMC departure.

The inspection should therefore report enough information to evaluate both the size requirement and the LMC-controlled geometric requirement. A diameter measurement alone does not establish whether the feature passes its position requirement.

Common LMC Interpretation Mistakes

LMC is often misread when the feature size, material condition, and geometric tolerance are treated as separate requirements. The easiest way to avoid that is to identify the type of feature first, then read its size limits and the modifier together.

Assuming LMC Means the Smallest Dimension

LMC does not mean choosing the smaller numerical value on the drawing.

For a hole, the larger permitted diameter is LMC because a larger hole contains less material.

For a shaft or pin, the smaller permitted diameter is LMC because a smaller shaft contains less material.

For example:

• Hole: Ø10.00 ±0.05 mm → LMC = Ø10.05 mm
• Shaft: Ø10.00 ±0.05 mm → LMC = Ø9.95 mm

The feature type determines which size limit represents LMC.

Confusing LMC With Size Tolerance

LMC is not another size tolerance.

A callout such as Ø10.00 ±0.05 mm still controls the actual feature size. If an Ⓛ modifier is added to a geometric tolerance, it changes how that geometric requirement is evaluated in relation to the feature's LMC condition.

So, when checking a drawing, keep these two requirements separate:

• Size dimension: controls how large or small the feature can be.
• LMC modifier: establishes the material condition used for the related geometric requirement.

Least Material Condition FAQs

Conclusion About Least Material Condition

Before adding an Ⓛ modifier to a drawing, define the actual condition that needs to be protected, such as a minimum edge distance, wall thickness, or material between two features. The LMC requirement should then match that functional limit and the inspection method available for the part.

For production, the drawing should give the supplier the feature size limits, geometric tolerance, datum references, and LMC modifier needed to inspect the feature correctly. If those requirements are unclear, the LMC callout alone does not resolve the manufacturing requirement.

Have an LMC-controlled feature on a CNC part? Send the drawing to JLCCNC for a DFM and GD&T review before machining.