Tutorial - Creating Multi-element Heterogeneous device Symbol in Proteus ISIS

In today’s tutorial we will learn “How to make  multi-element heterogeneous device symbol in Proteus ISIS”. The image on the left shows a device symbol consists of 7 elements where each elements have different number of pins.

We will make this 7 elements device symbol for NXP Semiconductors ARM Based Microcontroller LPC2478 using Proteus ISIS 8 demo version.

Why make Multi-elements heterogeneous device symbol instead of One single element symbol?

The answer to this question in my opinion is, its easy to deal with multiple elements of a device when it have hundreds of pins. So we split the device symbol into multiple elements which eases capturing our schematic.

Lets start our work to make one such symbol.

We will be making device symbol for LPC2478. LPC2478 is a 208 pin device available in LQFP as well as BGA package. We will make device symbol and then assign LQFP Package, You can also assign BGA Package to the symbol the process is the same. Datasheet of LPC2478 can be downloaded from here 

Proteus 8 Demo Version can be downloaded from Lab Center Electronics Website if you don’t have it.

Step 1 – Opening Proteus ISIS

Open Proteus 8 and click on the ISIS icon in the toolbar to open ISIS.

Step 2 – Make The first element in the multi-element device Symbol

Make device symbol for the Power part of the device. Assign names to pins and don’t assign number at this stage, we will assign numbers in the Package Assigning step. Select the symbol and invoke the Make Device tool using the toolbar button. In the warning window click OK, The Make Device window appears. In case you don’t know how to make device symbol in Proteus ISIS, read the tutorial Making Device Symbol in Proteus first.

Step 3  - Naming elements of the multi-element symbol package

In the Name Device field write LPC2478:A (<Name of Device> : <A,B,C….Z>), write U in the Reference Prefix field click Next

The Next Dialog says package cannot be assigned (we will do that later) click Next. Add datasheet if you want, select Category, subcategory, Manufacturer etc. for the Device, Select a Library and Hit OK to finish the dialog. We have created and saved the first element of Heterogeneous multi-element device symbol.


 

Step 4 -

Repeat Step 2 and Step 3 for all other parts, assign names as LPC2478:B, LPC2478:C and so on. Now you have complete device in different elements. We will assign a package to it in the next step to complete the tutorial.

Step 5 – Assigning Package to the multi-element device symbol

Add one instance of each element to the work area in ISIS. Select all and invoke the Packaging tool from the toolbar as shown in the image below

In the dialog that appears click add to add the PCB Package(footprint) of the device. To know how to create a device package in ARES read the tutorial Making Device Package in Proteus ARES

The Package assignment is not finished now. remember we didn't assigned numbers to pins while making symbols for them, here we have to assign numbers to the pins. The pin number assignment is time consuming process in making multi-element heterogeneous device symbol as you have to refer to the datasheet.

In the next window we have a column for each element and we will write the pin numbers in each column for the pins shown in the left most column, After assigning writing pin numbers in each column click Assign Package to finish.

This completes the tutorial. In this tutorial we have learned how to make multi-element device symbol in Proteus ISIS. Please feel free to comment for questions and suggestions.

Read More

Tutorial–Panelizing/Merging Different PCBs in Proteus ARES

Merging different Prototype boards on a single Panel and generating Gerber Files for it, So that we can submit a single job to the PCB Manufacturer.

Note:  This Tutorial applies only to double sided PCBs.

 

Contents

Introduction

Step 1 – Setting to Work

Step 2 - 4 – Viewing Gerber Files in Penalization mode

Step 5 – Arranging Boards on the Panel

Step 6 – Generate Gerber Files for the Panel

Conclusion

Introduction

Penalizing PCBs is the process of merging the Gerber files generated by a PCB package for different circuit boards in order to submit a single job to the PCB manufacturer. In this Tutorial we will merge Gerber files generated by Proteus ARES for three different boars. Proteus ARES generates Gerber files in RS-274X extended Gerber format. You can read about RS-274X and other Gerber formats at Wikipedia or somewhere else on the internet.

I assume you are familiar with schematic and PCB designing in the Proteus Design package. You can download the current free version of Proteus here. For this tutorial I used Version 7.7.

For this tutorial I am using three the Sample Project. I have previously generated the Gerber files for them in different folders for the sake of clarity

Project1-Gerber

Project2-Gerber

Project3-Gerber

Now we do the following steps to Panelize the Boards into a single Panel.

Step 1 - Setting to Work

Open the Proteus ARES Program. Set the Work area to the size of the Panel. Here are some tips for selecting the size of the panel

1. Know the dimensions of your boards
2. How many copies of each board you want?
3. What size Panel the PCB manufacturer can make(some PCB Manufacturers have restrictions on the Panel size some have not confirm it first).
4. Select the Panel size so that you can optimally place your boards without wasting much space on the Panel.

Now you are ready to set the work area go to the windows menu and select the option “Set Work Area” enter the dimensions of the Panel and Hit Ok.

Step 2 – 4 – Viewing Gerber Files in Penalization mode

Step 2 -

Now it’s time to open all the Gerber File we have previously created in ARES. Click the Gerber Viewer icon in the toolbar or Find it in the Output drop-down menu, the Gerber View window appears, navigate to the project folder and open the GERBVIEW for the first project as shown in the figure.

Step 3 -

After clicking Open, In the next popup window don’t forget to check the option “Penalization mode” as shown. Click OK

We have just viewed Gerber Files for the First Project in ARES in Penalization mode.


 

Step 4 -

Follow step 2 to Step 3 for the other two boards.

Note: “Don’t move any of your board until you do the process for each board you want to be on the Panel”. If you move a board and then try to load another you will get the option to save your work, it doesn’t matter whether you save or not you will get the other board in new work area, which we don’t want here. So be careful

 

Step 5 – Arranging Boards on the Panel

Now that you have loaded all of your boards to the work area, it’s time to arrange them on the Panel.

If you want to make a copy of a board you simply select it right click and select “Block Copy” place it as many times you want and then click escape key to end.

I arranged the Boards as shown in the below image


 

Step 6 – Generate Gerber Files for the Panel

Now we have to generate Gerber files for the Panel which has our three Board on it, these are Gerber Files you will submit to the PCB Manufacturer. The Steps to generate and save the Gerber Files for the Panel are as below (in the image)

Conclusion

Trick:
If you are having difficulty moving the boards, try to hide some layers.
This concludes the Tutorial.

Read More