pad shape edit

[pgo48]

HI, I have just started using ultiboard and I have a few questions

when I go from multisim to ultiboard is there a way to preview the package in multisim so I don't have to manually re-size it in ulti-board? This is very time consuming...

I find the pad sizes for IC's are too small. Is there a way I can quickly change the size and shape of all the pins on an IC and save that component so every time I use it it's the same?

[Sharanya_R]

Hello,

To clarify you would like to preview a the circuit in Multisim before transfering it to Ultiboard and you would like customize a component and save it.

You be able to preview the footprint of the component in Multisim, if you double click the component, select Edit Footprint, and choose Select from Database.  The dimensions are not given in Multisim, however you can change them in Ultiboard.  If you are familiar with the name of the footprint, some manufacturers place the dimensions within the footprint name or you can check the datahsheet of teh component for the dimensions.

In order to create a customer component in Multisim the following tutorial will be of assistance;

Creating a Custom Component in NI Multisim

After creating the custom component in Multisim you can custom Ultiboard landpattern for layout;

Creating a Custom Component in NI Ultiboard

You will be able to do the following;

• Creating a database group
• Defining a custom PCB part
• Setting the environment grid spacing
• Placing SMD landpattern pads
• Setting the Reference ID and Value
• Using the Ruler Bars for Object Positioning
• Defining the IC Package
• Creating the 3D Model
• Saving the landpattern to the Ultiboard and Multisim database
• Associating a landpattern with a Multisim symbol

If I can help you with anything else, please let me know.

[_user32]

pgo48

Here are a few useful links that may help you.   Some PCB layout people have the philosophy of always creating your own PCB footprint, and although I think this can be an ok strategy, I think however for most footprint / landpattern shapes you can reuse most of the existing Ultiboard information to your advantage.

Here are my recommendations:

1. Understand the IPC naming convention, (as over 1500 new standard IPC SMT footprints were added in v11 to accomodate new part creation).

http://landpatterns.ipc.org/IPC-7351BNamingConvention.pdf

IPC Type + Pitch(P) + Lead Span Nominal(X) + Height - Pin Quantity    - all units in millimeters (mm)

Here is a useful link that we put together mapping many of the common JEDEC / EIA industry names to the IPC equivalent(s).

http://www.ni.com/white-paper/11669/en 

2. Locate the Ultiboard footprint shape(s) in the database that you think may be appropriate (Place -> From database...).

a) Surface Mount ICs, in the database go to: Ultiboard Master -> Surface Mount Technology -> IC

b) RLC parts go to: Ultiboard Master -> Surface Mount Technology -> Resistor -> Chip [or SMD R&C]

c) Caps can be here: Ultiboard Master -> Surface Mount Technology -> Capacitors -> Chip [or SMD]

3. Have a new project window in Ultiboard open and just place a few of the shapes that you think may be a match for the new part that you are creating in Multisim. 

4. Verify the pad and footprint shape information against the datasheet.  

Tip -> The dimensioning tools are very good for this type of checking in Ultiboard (Click on Mechanical Layer and select (Place -> Standard Dimension).  Double click on the placed dimension to adjust the displayed unit settings ("Other" object selection tool needs to be active).   For general layout I also usually set my standard copper grid settings to 1 mil or better to get fine dimension/copper measurement readings (Options -> PCB Properties -> Grid&Units(tab) -> Copper Grid -> 1.00000 mil (or better)).  However, in IPC checking, I find setting units to mm and setting the grid to 0.001 mm is best.

5. Once found and verified to match, open the footprint properties and note the SHAPE name in the attribute tag - this will usually be the primary Ultiboard name in Multisim.

Here is an example of some shape comparisons that I recently did for some various SOT-23 devices (note there is not just 1, there are multiple variations)...

6. If you don't find a PCB footprint that matches, you can modify the existing ones.   I prefer the "In-place part edit" feature (Ultiboard PowerPro only).   In this mode you can quickly make the modifications to the pad shapes, pitch or overall size and height and then save the part (File -> Save to database as...) and this will allow you to more easily create new parts (that are just slight variations of the existing parts).

Regards,

Pat Noonan