# How to edit dimensions for PCB layout in proteus

I need a relay like this in proteus

http://www.sanyourelay.ca/public/products/pdf/DI1U-K.pdf

the DI1U-P type.

unfortunately all the relay i found are not of the same size.

• Are you trying to make a suitable solder pad footprint, keepout area indication, or a model for the 3D render feature of Proteus? – Anindo Ghosh Jan 18 '14 at 6:54
• yes, .im trying to create a suitable solder pad footprint. – user35046 Jan 18 '14 at 7:11
• or just edit an existing one package to fit. – user35046 Jan 18 '14 at 7:11

This can probably be explained better in a in a video but I'll try with images

Open ARES and place a similar footprint on the design (a relay that matches the number of pins is fine)

what you get is

right click on the footprint and select decompose tagged objects

If the dimension of your footprint are in mm then pres the m button for metric or leave it as is for mils

use the 2D graphics mode to make the outline of the component (or resize the existing one) to match the one you are trying to create

change the snap size if needed, then use the dimension mode and create lines or use the grid or numeric coordinates to help you place the pads (move the existing ones from the decomposed footprint) to the appropriate distances as per the device datasheet.

when you are done select the created footprint (pads & outer line) plus the text from the decomposed component (this helps avoid entering everything from scratch), right click and select make package

in the next screen use a new name and change any other info you may want (not required) and store the new footprint in a user library like USERPKG

In order to use the footprint in your actual PCB that is connected to a schematic you can double click the relay component and change the footprint name to match the new one you have designed, so this

is changed to

Another option is to change the linked package to the ISIS schematic editor.
Place a component that has the same number of pins (and names, or you have to do additional steps), right click and select packaging tool

select the package you have created

Set the footprint to schematic pin names association if necessary (not needed if names match) , set it as default (assuming you don't want to set it every time) and click assign package

then save it in a new library like USERDVC.

Note that after that you'll have two relays with the same name with one of them belonging to the USERDVC package, that is the one you should use

If you need a video tutorial then there are a few in youture, like https://www.youtube.com/watch?v=CHowCns-8IU

• I really need this.thank you so much! ! ! it appears my only problem was the snap size because the measurements where like 40th 10th like that and I did not know what those mean. Now its in mm thanks you so much! Solved my problems – user35046 Jan 19 '14 at 14:31
• @user35046 The snap setting only sets the minimum step distance of the cursor, your problem seems to have been the actual units used. FIY a mil is a thousandth of an inch (1/1000 of an inch). There are many components that use dimensions in mils, for example standard dip IC have a distance of 100mil between two pins, SOIC have 50 mil between pins etc. – alexan_e Jan 19 '14 at 14:48

You can modify one of the footprints or create your own. To do that you need to create a library in proteus. Go to the PCB editor(I think it was ARES) and create a user library from the libraries menu. Next you can place the footprint from a similar package and right click on it and click decompose(or something similar I can't remember the exact name). This will split the component into its constituents e.g. pads, top silk etc. You can then modify the component, select all parts by dragging over it and right click and create new footprint. You just need to go through the wizard and make sure to select the new library.

P.S. If you save the library in a directory outside the library path, you may need to add it to ISIS and ARES. Paths was in one of the last menus, if I remember correctly.