This website requires JavaScript.

User Guide to the JLCPCB Impedance Calculator

User Guide to the JLCPCB Impedance Calculator

The JLCPCB Impedance Calculator computes track width values and recommended stack-ups from user-input values of board thickness, copper weight, layer, target impedance, conductor spacing (for edge-coupled pairs), and conductor-to-ground gap (coplanar waveguides).

User Interface

1. Layers: Total number of copper layers in the board.

2. Finished Thickness: Thickness of the finished PCB, including soldermask.

3. Internal Copper Thickness: Copper weight for internal layers. The calculator only supports 0.5 oz and 1 oz; for calculations with 2 oz internal copper please contact customer support.

4. External Copper Thickness: Copper weight for the top and bottom layers. Although JLCPCB can produce boards with 2 oz external copper, the calculator only supports 1 oz because (1) the wider tolerance of 2 oz traces hinders impedance control, and (2) most signal traces only carries small currents.

5. Unit: Options are mm, mil, μm, and inch.

6. Impedance (Ω): The desired impedance. The range of accepted values is 20 to 90 Ω for single-ended and 50 to 150 Ω for differential signals.

7. Type: Options are microstrip (single-ended), coplanar (single-ended), edge-coupled (differential), and dual coplanar (differential). Make sure the correct Layer is selected before changing this option.

8. Layer: Which layer the signal should be on.

9. Reference Layer Above: Only needed if the signal is on an internal layer.

10. Reference Layer Below: Does not need to be one layer below the signal; for example for a signal on L3, this option can be L4 or L5. However there must be a ground plane associated with the signal on the reference layer selected.

11. Conductor Spacing: The gap between the two conductors in a differential trace. Increasing conductor spacing increases the calculated trace width.

12. Conductor-to-Ground Gap: The gap between the signal conductor and the surrounding ground in a coplanar waveguide configuration.


· The first stack-up recommended by the calculator usually has the lowest cost and quickest turn-around.

· The 3313 prepreg replaces the previously available 2313. Their thickness and dielectric constant (εr) are the same.

· For the same nominal copper weight, internal layers have a slightly smaller thickness than external layers due to a small amount of copper being lost in production during deoxidation etc. For example, 0.5 oz copper on internal layers is 15.2 μm thick 4- to 8-layinstead of the nominal 17.5 μm.

· Results for 4- to 8-layer boards are calculated assuming Nan Ya Plastics NP-155F core material, and SYTECH S1000-2M for 10-layer boards and higher. The correct material should be selected when ordering so that the calculated parameters give accurate impedances.

Calculation Parameters Used

External copper thickness (1 oz)1.6 mil
Internal copper thickness (0.5 oz)0.6 mil
Internal copper thickness (1 oz)1.2 mil
Base soldermask thickness1.2 mil
Copper-surface soldermask thickness0.6 mil
Soldermask thickness in between traces1.2 mil
Soldermask dielectric constant (εr)3.8
Trace top widthTrace base width – 1 mil

Nan Ya Plastics NP-155F (4 to 8 layers)

Core ThicknessεrPrepreg TypeResin ContentNominal Thicknessεr
0.08 mm3.99762849%8.6 mil4.4
0.10 mm4.363313 (2313)57%4.2 mil4.1
0.13 mm4.17108067%3.3 mil3.91
0.15 mm4.36211654%4.9 mil4.16
0.20 mm4.36
0.25 mm4.23
0.30 mm4.41
0.35 mm4.36
0.40 mm4.36
0.45 mm4.36
0.50 mm4.48
0.55 mm4.41
0.60 mm4.36
0.65 mm4.36
0.70 mm4.53
> 0.70 mm4.43

SYTECH (Shengyi) S1000-2M (10+ layers)

Core ThicknessεrPrepreg TypeResin ContentNominal Thicknessεr
0.075 mm4.1410672%1.97 mil3.92
0.10 mm4.11108069%3.31 mil3.99
0.13 mm4.03231358%4.09 mil4.31
0.15 mm4.35211657%5.00 mil4.29
0.20 mm4.42
0.25 mm4.29
0.30 mm4.56

The values provided above are for reference only. Some of the values have been calculated from test results by JLCPCB and may be adjusted in the future.

Stack-Up Naming Scheme

Last updated on Aug 25, 2023