Unit Conversion and Component Measurements in PCB Design

Question

I’m working on a PCB project and need to ensure that the components match their respective datasheets. I encountered an issue where one of the components I’m checking was created by someone with units in mils. For example, I noticed that a dimension listed as 0.40 mm in the recommended footprint from the component's datasheet is represented as 14 mils in the created footprint. I understand that the difference is minimal, as 0.40 mm is approximately 15.748 mils.

I’m considering switching the units to mm and correcting the values in the library, but I’m unsure if this is the right approach. So, I’d like to ask: if a component is created with measurements in millimeters and another in mils, and the PCB designer uses mils for the board layout, could this cause any issues or difficulties for routing or other aspects? Also, what is the best way to round or convert measurements between units? Should I consider significant figures or the manufacturing process (and if so, how)?

I’m using Altium Designer and I know that it’s possible to switch between units, but I’m unsure if it’s recommended to switch units during the PCB design process.

Answer 1

In comments on another answer, you clarified your question:

it seems like the person who created the library made the footprint with slightly different dimensions than those in the datasheet. ... I understand the difference is small, but I don't understand why they did it this way—if there was a specific reason for it.

It's hard to answer this without knowing what dimension it was. For example, making a pad longer (in the axial direction) might have been done to make it easier to hand solder.

Up to a point, there is also a trade-off between enlarging the pads to reduce assembly defects and reducing them to allow packing components more tightly on a board.

If you want to make a good choice of dimensions that is likely to be usable across a wide range of assembly vendors, then it is a good idea to invest in and follow the recommendations in IPC-7351, a standard produced by the Institute for Printed Circuits. Even following IPC-7351 you are given different choices for the patterns depending on the relative importance of reducing footprint size vs minimizing assembly defects in your project.

They used measurements in mils, but the datasheet is in millimeters.

The difference between mils and millimeters should be immaterial, as long as they are using enough decimal points. Below about 0.1 mil or 0.0025 mm, any difference in copper or solder mask dimensions will typically be insignificant due to manufacturing tolerances.

Answer 2

So, I’d like to ask: if a component is created with measurements in millimeters and another in mils, and the PCB designer uses mils for the board layout, could this cause any issues or difficulties for routing or other aspects?

It really depends on what your boardhouse can do with tolerances and linewidths. Most will have some spec like 0.5mil (which is 0.0254mm) so even if you do correct that 0.3mil error (~8um) it really won't matter because most PCB's are not be fabricated to such a small spec.

It can create some small issues for DFM, for example: If I had BGA pads that needed to be exactly 9mil apart so you can fit a 3mil trace between with 3 mil on either side and you increase the size of the pads to 3.2mil, then the DFM rule of 3mil clearance will be broken, and you won't pass DFM in the PCB design software. But for normal PCB's (not HDI) one does not usually need to worry about this (and it can be fixed with rules or exemptions anyway)

Also, what is the best way to round or convert measurements between units?

I usually use 2.54cm per 1 inch. If you are rounding it only matters in terms of tolerances so unless your design has a 10um or less grid, I wouldn't worry about it. It's fine to switch between units in altiuim, I've never had an issue and do it on a regular basis.