LIBRARY PARTS

Introduction

The Proteus Design Suite comes with a significant installed base of schematic components, almost all of which are already packaged with the correct PCB footprint. However, with the number of new parts entering the market every day and the vast choice available to engineers it is inevitable that users will have to either import library parts into Proteus or create library parts inside Proteus.

Importing Library Parts

There are three ways to get hold of a part that is not in the installed libraries: import a ready-made one, ask the AI assistant to build one, or draw it yourself. They are worth trying in that order.

Importing is much the best option wherever it is possible. It is far quicker than drawing a part by hand and considerably less error prone, and it brings in the schematic component and the layout footprint together. Proteus supports two routes for import:

  • Integrated Web Search and Import (requires a valid maintenance contract)
  • Manual Library Part Import Dialogue.

If nobody has made the part you need, the next thing to try is the AI assistant, which can construct a symbol and a footprint from the datasheet. Drawing a part by hand is the last resort; all three routes are covered in the sections that follow.

Short tutorial videos on working with both import methods can be found on our Youtube Channel

Web Search Import

The integrated web search import works directly from the Pick Devices dialogue form. You simply type the part name you want and, after searching the installed libraries, you can search a database of over 15 million parts from our partners Samacsys & SnapEDA. Just click on the provider that you wish to use! This service requires a free account to be registered with Samacsys / SnapEDA and a valid maintenance contract to import the parts.

Searching the partner parts database from the Pick Devices dialogue form

Library Part Import Dialogue

This method enables you to manually import via the Import Parts command on the Library menu in either the schematic or the layout editors. This import will work with all major vendor files such as those generated by Ultra-Librarian, Samacsys, SnapEDA and PCB Library Expert as well as through common supplier portals such as Digikey or RS Components. It does not require a valid maintenance contract to work but does involve slightly more effort.

The Import Parts dialogue with a part loaded.

The Import Parts dialogue with a part loaded.

Technically, the import works with PADS Library V9.x files, meaning that the import will work with any supplier who can generate a fileset in this format.

To import a library part using the Pick Devices dialogue form

Web search import works as follows:

1) Launch the Pick Devices dialogue form in the schematic module (also 'P' on the keyboard).

The P button above the Object Selector in the schematic capture module

2) Search for a part. If matches exist in the installed libraries they will be shown and you can click to open web search results from the bar at the bottom of the Pick Devices dialogue form. If there are no matches from the installed libraries you will go directly to web search results.

The Pick Devices dialogue form with the web search bar at the bottom

3) Results in normal font are available for import. Results in disabled text can be requested (at no charge) from the build service form.

Web search results, with the parts available for import shown in normal font

4) Double click to import. The first time you do this you will need to supply credentials or create a free account.

The import confirmation prompt and the authentication dialogue for downloading parts

5) When you double click to import, both the schematic part and the associated PCB footprint will be brought into your user libraries and also picked into the current project. In most cases, the 3D STEP file for the footprint will also be imported.

The imported part shown in the Object Selector

If you need to request a part to be made you can do so directly from the pick dialogue by double clicking on one of the disabled entries in the web search. The service is free of charge and average turnaround is 24-48 hours.

Requesting a part to be made from a disabled entry in the web search results

To import a library part using the dialogue

1) Download the part you want onto your computer. This will almost always be in a zip file.

Saving the downloaded part as a zip file

2) If the part doesn't come from a vendor source that we directly support (see here) then you'll need to extract all the files from the zip into a folder of your choice.

3) From the Library menu in Proteus select the Import Parts command

The Import Parts command on the Library menu

4) Click on Select File and use the file selector on the right hand side to select either generic PADS Library V9 files or the vendor of your choice.

The file selector with Ultra Librarian chosen from the list of vendor formats

5) Choose the appropriate file to load. This will normally be a zip file if the vendor is selectable in the file selector or a .p file if you've had to extract the parts into a folder.

Choosing the file to load in the Import Parts dialogue form

6) Review the parse log and the previews to make sure everything looks good. Use configuration settings if need be to fix problems.

The parse log and previews shown after loading the part file

7) Use Import Part and follow the wizards to bring first the footprint and then the component into Proteus. This will both put the parts into your libraries and deposit them in the parts bin of the current project ready for placement. You should have an end parsed result that looks like the following:

The import log confirming the PCB package and schematic decal have been imported

What you are actually doing at this last stage is running the Make Package tool to create the footprint and then running the Make Device tool to make the schematic component. The areas where input may be required from you are in the library choice and the description and categorisation of the part.

For most complex devices, you can also find a BSDL script from the manufacturer. This is schematic part only but can be imported via the same Import Parts command (select BSDL in stage 4 above).

If neither import route turns up the part you need, the next section covers having the AI assistant build it from the datasheet instead.

Creating Parts with the AI Assistant

If the part you need does not exist anywhere, and you have configured the AI assistant with your own model and API key, ProPilot can build it for you. This is the route to reach for when importing a ready-made part has drawn a blank. Open the chat side bar with the ProPilot (AI Assistant) command on the Help menu, describe the component you want, and ProPilot will generate a schematic symbol, a PCB footprint and the part definition that ties the two together. It searches the installed libraries for a suitable symbol and the IPC-7351 library for a matching package before it constructs anything from scratch, so more often than not the result is assembled from material that is already known to be good.

What ProPilot needs from you is the information on the datasheet: pin names, pin numbers, electrical types and the recommended land pattern. The most effective way to hand that over is by screenshot. Use WIN+SHIFT+S to grab the pinout table or the land pattern drawing from the datasheet, then CTRL+V to paste it straight into the chat. Take the pages you need one at a time rather than attaching the whole PDF; a 50 page datasheet gives the model a great deal more to wade through than it needs, and the results get worse rather than better.

Worked Example: the MCP23008

Let us build a Microchip MCP23008 I2C expander. This is deliberately the same part that the appendix which follows builds by hand, so you can work through both and compare the two routes.

Start the conversation with something like:

"I need a library part for the Microchip MCP23008 I2C expander. I'll paste in the relevant datasheet pages."

ProPilot will ask for whatever it still needs, typically the pinout and the package dimensions. Grab the pin diagram from the datasheet and paste it in, then do the same for the recommended land pattern of the package you intend to use.

The pin diagram from the MCP23008 datasheet pasted into the ProPilot chat

The pin diagram from the MCP23008 datasheet pasted into the ProPilot chat.

Attaching the full datasheet can eat a lot of tokens as Propilot will read the entire datasheet, and it doesn't need half the information to make the part. This will cost you money that you don't need to spend!

ProPilot parses what you have given it, looks for an existing symbol and package, generates the part and submits it to the same Import Parts dialogue we used for the import routes, this time for preview. That dialogue is modeless, which is the key to the whole workflow: it stays open alongside the chat, so you can inspect the symbol and the footprint, read the dimensions off the preview, and then go straight back to the chat to ask for a change. The MCP23008 gives you a fair amount to look at, with eight GP pins, three address pins, the I2C pair and a RESET pin that wants an overbar.

The Import Parts dialogue previewing the generated MCP23008 symbol and footprint, with the ProPilot chat alongside

The Import Parts dialogue previewing the generated MCP23008 symbol and footprint, with the ProPilot chat alongside.

If something is not right, leave the dialogue open and type the correction into the chat: name the dimension that is wrong, ask for a different library footprint, or ask for the pins to be arranged differently. ProPilot regenerates the part and the preview updates in place. There is no limit on how many rounds you go and each correction builds on the previous version, so nothing is lost by iterating. Expect to iterate; the workflow is designed around it.

The regenerated MCP23008 preview after a correction typed into the ProPilot chat

The regenerated MCP23008 preview after a correction typed into the ProPilot chat.

When both the symbol and the footprint look right, click Import Part. Nothing is written to your libraries until you do, so a part that has gone badly wrong can be abandoned simply by not importing it.

Checking the Result

ProPilot runs its own checks, but a human review catches things an automated one cannot. Before you click Import Part, run through the following:

  • Do all the pin names match the datasheet exactly?
  • Are the pin numbers correctly assigned, rather than shifted or mirrored?
  • Are inputs on the left of the symbol and outputs on the right?
  • Does the footprint pad count match the component?
  • Do the pad size, pitch and span match the recommended land pattern?
  • Is the silkscreen clear of the pads?

Always verify the footprint against the land pattern on the datasheet before importing. ProPilot is highly capable but a wrong footprint is one of the expensive mistakes in PCB design and the bill for it is a board respin. Spending 30 seconds checking pad size, pitch and span now can save days later.

What arrives in your library from this route is an ordinary Proteus library part, with nothing special about it. If you would like to understand what ProPilot has done on your behalf, the appendix that follows builds the same MCP23008 from a rectangle and a set of pins.

See Also:

Library Part Creation with ProPilot (Reference Manual)

Creating New Devices

If all else fails you can create parts  yourself entirely inside Proteus. Alternatively, you may wish to permanently adjust the properties or footprints of an existing component. This section of the documentation starts from the basics of creating a new device and covers the entire process through to storing the new part in the library.

While the following topics are a detailed explanation of how to create component parts in Proteus, in practice this should almost never be necessary. In addition to the many installed libraries Proteus includes a web search with access to 15 million library parts, and the universal part importer provides support for almost all third party part vendors (Ultra-Librarian, Samacsys, SnapEDA, etc.). If the part doesn't exist in Proteus itself the next step is to search for it and import it directly from a third party vendor, which is discussed in some detail in the importer help file and shown on our Youtube Channel. If that draws a blank too, and you have the AI assistant configured, the previous section shows how to have ProPilot build the part from the datasheet. Drawing a part by hand, as we do below, is genuinely the last resort.

Graphics and Pins

For our example part lets assume that we want to create a Microchip MCP23008 I2C expander. The first thing we need to do is to create a graphical representation of the part on the schematic. When we are finished it should look something like the following:

The MCP23008 Completed

The MCP23008 Completed

Let’s begin by placing the component body as follows:

  • Select the 2D Graphics Square icon and make sure the component style is selected in the Object Selector.

The 2D Graphics Square icon with the component style selected in the Object Selector

  • Left click once on an empty area of the schematic to begin placement.

A rectangle being sized on the schematic during placement

  • Move the mouse until the rectangle is around the size of the part that you want. It’s better to make this slightly larger than might be required as we can easily resize it later.
  • Left click again to complete placement of the graphic.

The placed component body graphic

Proteus supports a powerful graphics style system of local and global styles and the ability of local styles to follow or track global styles that allows you to easily and flexibly customise the appearance of your schematic. See the section Graphics and Text Styles in the online reference manual for a complete explanation of how styles work and how they are used.

The next job is to place the component pins.

Select Component pin mode and make sure that you have the default pin type selected in the Object Selector.

Component pin mode with the default pin type selected in the Object Selector

  1. Left click the mouse on the schematic to begin placement. The small cross at the end of the pin indicates the side of the pin that will be wired to so it is important that this is outward facing.

    A component pin being placed, with the cross at its outward facing end
  2. Move the mouse so that the other end of the pin touches the edge of the component graphic and left click again to place

    A pin placed against the edge of the component graphic
  3. A new pin is automatically primed for placement so simply move the mouse down slightly and left click to place again.

    Pins placed down the left hand side of the component graphic
  4. Repeat the process down the left hand side of the component graphic using the completed screenshot as a reference. Right click to finish placement.
  5. Click on the X-Mirror icon to point the pin in the opposite direction ready for placement down the right hand side.
  6. Repeat as of stage 3 to place the pins down the right hand side of the component.
  7. Right click the mouse when you are finished to exit pin placement mode.

The Plus (+) and Minus (-) keys can also rotate the pin during placement, but you will find that when adding pin numbers, they will be on the opposite side of the pins that you placed before rotation. In this case right click on the pin(s) affected and click the Y-Mirror option to correct the pin(s).

Two pins placed facing in opposite directions

At this stage your component graphics should look something like the following:

The body of the MCP23008

The body of the MCP23008

The actual positioning of the pins is of course somewhat aesthetic and you may prefer to have different groupings to those we have chosen.

Now that we’ve placed the pins we may need to adjust the size of the component body to fit them better. To do this, click on the Selection Mode icon and left click on the edge of the component body, then left depress the mouse on one of the nodes, drag to the new size and release the mouse to commit.

This works much like any other graphics package. If you pick up a node along the bottom edge you can drag up and down; pick up a corner node and you can drag diagonally. Make sure however, that you do not leave any of the pins ‘hanging’ (not touching) when you do this, else you will have to subsequently move the pins back onto the component edge.

If you want to make fine adjustments you may need to adjust the Snap level – these options are available from the View menu (defaulted to 0.1in) and are discussed in more detail in the reference manual.

Now that we have the basic shape of the part we need to add names to the pins. This can be done as follows:

  • Right click on the pin at the top left of the component and select Edit Properties from the resulting context menu.

The pin context menu with the Edit Properties command

  • Type in the name of the pin (SCL), the default pin number (1) and the electrical type (INPUT). You can use the other options to control visibility but for our purposes the defaults are fine.

The Edit Pin dialogue form with the SCL name, pin number and electrical type entered

  • Hit the Next button at the bottom to switch to the next pin in the list and repeat the process – the schematic will update to show which pin you are editing. If you are unfamiliar with this part and don’t therefore know the electrical type of the pin simply leave it as the default Passive type.

The Electrical Type options for a pin, with Passive selected

  • When you get to the RESET pin you’ll need to add an overbar. Do this simply by adding a dollar (‘$’) prefix and suffix to the name.

The RESET pin name entered with dollar signs to add an overbar

  •  Hit the OK button when you are finished.

You may have noticed that there is a significant omission from the schematic part as we have drawn it so far, namely that there are no physical power pins on the device. Since we do not need to wire power nets explicitly we do not need a physical pin for the component. We need only ensure that the power pins are handled correctly with respect to the physical PCB footprint and we’ll discuss this in more detail in the next section. It is worth noting however, that while it is very common to have non-physical power pins in order to reduce clutter on the schematic, you may have a preference for everything to be explicitly wired. In this case you could simply add two extra pins and name them VDD and VSS respectively.

Our final task now is to make a device from the composite graphics and pins that we have placed. Start by drawing a tag box around the entire graphic (left depress the mouse and drag out the selection box). Next, right click the mouse inside the selection box and select the Make Device option from the resulting context menu.

You will notice Group Objects and Ungroup Objects further down that same context menu. They do something quite different: grouping keeps a set of objects together on the schematic, as we did with the blocks of circuitry earlier in the tutorial, whereas Make Device turns the graphics and pins into a single library part. Make sure you pick the right one here.

Make Device icon and the Context menu option

Make Device icon and the Context menu option

This presents us with the Make Device dialogue form, where we can customise the part. All fields throughout this wizard have context sensitive help associated with them, accessed by clicking on the question at the top right and then on the field in question. However, the only items we need to deal with here are the Device Name and the Reference Prefix. The device name should be MCP23008 and the reference prefix should be ‘U’.

The reference prefix serves to categorise parts for Bill of Materials Output and is also used in annotation. These are fairly standard across the industry with ‘R’ denoting resistors, ‘C’ for capacitors, ‘U’ for IC’s and so on.

Use the Next button at the bottom of the dialogue to move onto the next screen.

Adding Footprints

In a previous section of the documentation we saw how to quickly add a footprint to a schematic part. This is useful for small passives and simple parts but, when we are creating a device we need to follow a more complete procedure. This ensures not only that we have a correct mapping between the pins on the component and the pads on the footprint but also allows us to better handle power pins.

From the screen on the Make Device dialogue form click on the Add/Edit button to launch the Visual Packaging Tool. The first thing we need to do is to find the footprint we want to use so click on the Add button at the top of the dialogue form.

The 'Add' button in the Packaging Tool

The 'Add' button in the Packaging Tool

This brings up the package browser dialogue which we covered earlier in the documentation. Assuming that we want the surface mount package, type SOP18 in the Keywords field and then double click on the part in the results list to select it.

Selecting the SOP18 from the package library

Selecting the SOP18 from the package library

The Visual Packaging Tool will now look something like the following screenshot.

The SOP18 footprint shown in the Visual Packaging Tool

There are several points of note here. Firstly, the pads in the preview which are white are deemed to be mapped onto component pins. This has happened as we have correctly specified the default pin numbers when we edited the pins earlier on (pad name maps onto pin number when present). If we had chosen to leave the pin number fields blank we would have to map all of the pins in this dialogue form.

Secondly, we can see that there are three pads (7, 9 and 18) which are not mapped onto component pins. Normally we would have the datasheet beside us to get the footprint mappings but in this case pin 7 is an NC pin, pin 9 is the VSS pin and pin 18 is the VDD pin.

The NC pin is easily handled – simply type 7 in the field for NC Pins. Notice that the preview on the right hand side will update to show that this pad is now considered dealt with.

We now need to add two ‘virtual’ pins for the power pins. These are pins which don’t need to be on the schematic (their connection is made implicitly according to their name) as they will add unnecessary clutter, but do need to be mapped onto pads in the footprint.

If you want to have all pins visible on the schematic (e.g. for auditing purposes) you can certainly do so. You would add another three pins to the device, connect one of them to an NC terminal (to put on the NC net) and connect the other two to power terminals with the correct names. If you are in any doubt regarding power nets and connections please see the section earlier in the document on powering the circuit or consult the reference manual.

Click on the Add Pin button underneath the grid, type VSS to name the pin and then repeat the process for the VDD pin. Remember that connections to these virtual pins are made according to their name so make sure that you name them correctly.

Adding a virtual pin

Adding a virtual pin

NC pads and virtual power pins are the fiddliest part of making a device by hand, and they are also exactly the part that the AI assistant reads straight off the datasheet. If you find yourself doing this often, it is worth trying the ProPilot route described earlier in this section and reviewing the result instead.

Having created the pins we assign them to pads on the footprint as follows:

  • Click in the column at the far right of the VSS pin.
  • Click on the corresponding pad on the footprint (pad 9).
  • The cursor will move down to the next pin (VDD) so all we need to do is click on pad 18 on the preview.

Clicking on pads will assign the pin

Clicking on pads will assign the pin

We should see that all the pads on the footprint are now highlighted, indicated that the part is fully packaged. Simply hit the ‘Assign Package’ button at the bottom of the Visual Packaging Tool to commit and return to the Make Device dialogue form.

It is possible (and extremely useful) to have more than one packaging for a given component. We could, for example, follow the exact same procedure to add a DIL18 footprint to the component. Where more than one packaging exists you can specify the one which will be used by default by checking the default box underneath the package name in the Visual Packaging Tool.

Click the next button at the bottom of the dialogue form to move onto the Property definitions section.

See Also:

Packaging Tool (Reference Manual)

Adding Properties

This screen allows us to add component properties to the device. We looked at doing this on a particular instance of a device (the part on the schematic) earlier in the documentation; the difference is that properties entered here will be stored in the master library part and therefore available every time we use the part in a design.

We can see that the PACKAGE property is already defined – this was what we configured visually on the previous screen

Package preview on the Make Device form

Package preview on the Make Device form

Let’s assume we want to add a property for RoHS compliance.

  • Start by clicking on the New button at the bottom left and then clicking on Blank Item.
  • On the right hand side fill out the name as ‘ROHS’ and the description as ‘RoHS Compliant’
  • The next field is the data type which in our case is a simple Boolean (Yes/No) – select this from the drop down list.
  • Change the Default value to be Yes and leave the visibility defaults as they are.

The component properties page of Make Device with a Boolean property defined

If you want to add more properties (e.g. MoQ, Price, Code, Supplier, etc.) simply repeat the process above.  Alternatively, the Bill of Materials provides a convenient way to apply data to schematics as discussed earlier in the tutorial. Finally, for complete control or if you are doing this on a large scale, we recommend you read up on ASCII Data Import in the reference manual.

Click the next button at the bottom of the dialogue when you are finished to move on to the next screen.

Attaching a Datasheet

This screen allows us to attach a datasheet to the part we are creating. To do this we would need to enter the filename for the datasheet and then configure the path as required. As we don’t have a datasheet handy we’ll ignore this step but the following screenshot shows an example of how we would set it up.

Adding a datasheet to the component

Adding a datasheet to the component

The main advantage of working through this step is to have the datasheet handy when you place the part. If present, you can simply edit the component and click on the Data button at the right hand side.

The Data button will launch the assigned Datasheet

The Data button will launch the assigned Datasheet

For convenience, we have configured many of our library parts with datasheets which you can download from our web server via this button.

If there is a data sheet that you want to use from the manufacturers or suppliers website, you can also add this. For example, find the URL of the datasheet:

https://ww1.microchip.com/downloads/en/DeviceDoc/MCP23008-MCP23S08-Data-Sheet-20001919F.pdf

and add as such:

The Device Data Sheet and Help File page of the Make Device wizard

Data Sheet Filename: MCP23008-MCP23S08-Data-Sheet-20001919F.pdf

Download Server: https://ww1.microchip.com

Download Path: downloads/en/DeviceDoc/

When you click on the DATA button in the Edit properties form, you will be told Datasheet not found, with an option to download it. Click on the Download button and it will pull it from the stated URL.

Indexing and Library Selection

The final screen allows us to categorise our part and choose which library we will place it in. As we have seen earlier in the tutorial the part description and the categories are used as filters when finding and selecting parts from the library so it is worth giving some thought to your description. An example of what you might enter is shown in the following screenshot.

Final section where you save the component to a library

Final section where you save the component to a library

When you are finished simply click the OK button. You will be prompted to replace all instances of the device on the schematic – this allows you to update the current design if you are modifying a part which already exists on the schematic.

Finally, if you now select the part from the Object Selector and edit it’s properties you should see something like the following screenshot.

Edit Component for the MCP23008

Edit Component for the MCP23008

It is also possible to create multi-element parts in Proteus. While beyond the scope of this tutorial these are covered in the reference manual.

See Also:

Creating Multi-Element Devices (Reference Manual)