0
\$\begingroup\$

I am new to the PCB world and currenctly I am using NI ULTIBOARD program.

So lets say I have this part cre2512-r001:

enter image description here

Does that mean that C=2.2 mm or 2 mm or 1.8 mm? becouse I am a bit counfused what is the size of the pads.

The same goes for A. Is A=6.65 mm or 6.45 mm or 6.25?

\$\endgroup\$
  • \$\begingroup\$ C will be between 1.8 and 2.2, nominally 2, but the +/- is the tolerance. \$\endgroup\$ – Colin Apr 17 at 9:52
  • 1
    \$\begingroup\$ The PCB pad sizes are going to be larger than the product pad dimensions; there is usually a suggested PCB dimension diagram or link in datasheets. \$\endgroup\$ – Peter Smith Apr 17 at 9:56
  • \$\begingroup\$ so basically I am allways using the deafult meaning the C=2 mm and A=6.45mm and B=3.35 mm and so on ... ? \$\endgroup\$ – Tomer Polski Apr 17 at 9:58
1
\$\begingroup\$

The data you are refering to are the Product dimensions. You should design your pad layout such that a component with minimum dimensions as well as a component with maximum dimensions will both fit, so both can always be decently mounted to the PCB.

For machine Placement/Oven soldering I would just use the the Recommended Solder Pad Layout as given in the datasheet. enter image description here

The picture right of the recommended Pad Layout is from my own (component) editor. Red are the pads, yellow the silk screen with the component drawn in the typical dimensions.
For this question, I added the component's minimum and maximum dimensions in grey as well, so you can see how both still fit into the recommended solder pad layout.
For manual soldering I would recommend to keep A and L as provided, but increase B.

Don't forget to apply the sensing traces as shown in your PCB editor. The Kelvin connection is required for a good measurement.

Nota Bene
In the datasheet, the letters A, B and C for the Recommended Solder Pad Layout differ (in meaning) from the A, B and C used for Product dimensions.

EDIT:
I updated the right picture, so you can see the pads of the component are still enclosed by the land pattern, even for the minimum product dimensions. L should therefore be 1.3 mm as recommended.

\$\endgroup\$
0
\$\begingroup\$

You have shared a package dimension. You need to make somewhat larger pads so that you can solder the part correctly. When it comes to deciding how much extra margin to take, it depends on the manufacturing process:

process

Since your component is pretty large, it should be easy to manage even for manual placement and soldering.

You can use the following dimensions:

package footprint

a = 3.5 mm

b = 5.0 mm

c = 2.2 mm

\$\endgroup\$
  • \$\begingroup\$ I am so sorry but I did not understand where you took this dimensions of a,b,c ?. As I understand your from your first pic ( I am doing MANUEL PLACEMENT MANUEL SOLDERING ) i need to A=6.65 mm B=3.55 mm and C=2.2mm all are the max Dimension ? \$\endgroup\$ – Tomer Polski Apr 17 at 10:18
  • \$\begingroup\$ a,b,c are from my personal experience. If you make the footprints with these dimensions, you will not face any challenge during placement and soldering. You can make the footprint a bit smaller or larger if you have reasons for the same. However my dimensions will work as a start. \$\endgroup\$ – Whiskeyjack Apr 17 at 10:44
  • 1
    \$\begingroup\$ ye but in the data shit A=6.45+-0,2mm how ever in your scheme A=c+b*2=2.2+5*2=12.2 mm meaning that in your scheme A is much bigger ... \$\endgroup\$ – Tomer Polski Apr 17 at 10:58
  • \$\begingroup\$ The minimum product length is 6.25 mm, the maximum plating length is 2.20 mm, so worst case the length between the terminals is (6.25-2.20-2.20 ) mm = 1.85. So, I think your c = 2.2 mm should be smaller. \$\endgroup\$ – Huisman Apr 17 at 11:51

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.