How to create schematic symbol and footprint for leadless chip carrier IC in altium designer | applied electronics engineering


How to create schematic symbol and footprint for leadless chip carrier IC in altium designer

By Applied Electronics - Friday, June 27, 2014 No Comments
Many times when you work with PCB design you need to create IC schematic symbol and footprint and possibly 3D model too. This altium designer tutorial shows how to create an integrated library of an LCC (leadless chip carrier) IC chip Quectel M10. Quenctel M10 is a wireless GSM/ GPRS module used frequently in electronics communication system. Integrated library means that schematic symbol, footprint and 3D model are integrated into a single library.

To start with, we gonna first create a new integrated library project, create the schematic symbol and then the footprint.

For those who want to directly see the 2nd part of the tutorial where footprint is created visit- LLC Footprint creation for M10 GSM/ GPRS module

To create a new integrated library project, select, File>New>Project> Integrated Library as shown below-

It is a good practice to save the files when they are first created. To save this integrated library project, right click on the integrated document file and select Save As and save the project in some suitable folder with some name in your PC.

Now we have to add the schematic library and PCB library to this integrated library project.

First we add the schematic library that allows us to create a new schematic symbol. To do this right click on the integrated library project icon and then select Add New to Project>Schematic Library.

To save this new schematic document, right click on it and select Save As and then save it with some name which will be automatically saved in the appropriate folder of this integrated library project.

Now we can start with the designing of the schematic symbol.

Click on the SCH Library button visible in the lower part of the panel part. Then you will see the component listed as Component 1 of the newly create schematic library.

 Now we want to rename this component. Select Tools>Rename Component and enter a suitable name.

Once you have completed the above steps the next step is to add the body and the pins.

It is easier to create the pins first and then the body because the when the body is first created, and then the pins added, we will come to situation of having to resize the body part again and again. Also with pins first created, it is easier to give the names to the Pins. On the other hand giving the pin names after creating the box can brings difficulty.

So lets add the pins firsts. For this you should know the pins names, number of pins required and the electrical properties of the pins. Usually you can see this in the IC Chip datasheet.

 To start with creating Pins, press P key twice or right click on the schematic and choose Place> Pin. A pin will be attached to your mouse cursor, click Tab key and it will bring up the Pin properties window. For now enter 1 in both the name and designator field and OK to confirm.

After this next pin with number 2 will be automatically attached to the mouse. Now keep on adding pins until there are 64 pins on the schematic.

Now we will make changes to the proper names of the pins. Open the Schematic List panel. If you don't see it then click on the SCH on the right bottom corner and then select SCHLIB List or from the View> Workspace Panel> SCH > SCHLIB List.

This list provides an easy way to rename the name of the pins. Right click on the Name column and select Switch to Edit Mode. By clicking on name of the first pin and rewriting the name from 1 to DISP_DATA and hitting enter will automatically choose the next Pin 2 where we can again enter the name for the second pin. By doing this we can rename all the pins quickly.

As shown by the following picture, the name has been changed-

Similarly we can change the electrical type of the pins by changing the Electrical Type column.

Now we will draw a box in the schematic editor and place 8 pins on its four sides. To place the rectangular box, right click onto the schematic editor and choose Place > Rectangle. Draw the rectangle onto the schematic editor.

Draw and attach the frist 16 Pins to the left side of the box. If the Pin names are not visible because the box obstruct them, right click on the box, go to properties and tick the transparent option.

Similarly, drag and attach the next 16 pins from 17 to 32 on the bottom side of the box. Once you select these 16 Pins you can rotate them by clicking the SPACE key.

Next drag and place the pins from 33 to 48 on the right side of the box.

Drag the box to align with the pins.

Finally drag and attach the remaing pins 49 to 64 to the upper side of the box.

Once the symbol creation is finished, we can give the designator name for the component, put some description for the symbol. For this open the properties window for the component and enter U? for the default designator, M10 as default comment and GSM module M10 as the description as shown below(you can give your own suitable comment and description).

This completes the creation of schematic symbol for our GSM M10 chip. It is advisory to now save all the files. Go to File> Save All to save the changes. The final schematic symbol looks like the following.

Next the PCB footprint for this component will be created using the IPC wizard option in altium designer.

Continue to 2nd part-  creating Footprint for LLC M10 GSM/ GPRS IC chip

No Comment to " How to create schematic symbol and footprint for leadless chip carrier IC in altium designer "