Win a 12 Month Licence to Altium CircuitStudio! - Review

Table of contents

RoadTest: Altium CircuitStudio! Roadtest

Author: michaelwylie

Creation date:

Evaluation Type: Independent Products

Did you receive all parts the manufacturer stated would be included in the package?: True

What other parts do you consider comparable to this product?: Altium Designer, Eagle, KiCAD

What were the biggest problems encountered?: Learning the ribbon style design.

Detailed Review:


This review is of the software package Altium CircuitStudio v1.2. My views are my own, and have not been paid for in any way. I was given a free copy of CircuitStudio to evaluate by element14. This review is late due to illness and the Holiday Season, and for that I apologize. Also, I cannot figure out why some images are fuzzy in the review. They're clear when I'm editing the document, but when I save it they go fuzzy. Happy reading!



If you don't want to read the whole review, just read this! I really like CircuitStudio for my needs. I need basic schematic capture and PCB layout software, and I like the price tag of $1000 vs the $7000 for Altium Designer. This review is for version 1.2, although 1.3 was released before the end of this RoadTest. What you might lose by using CircuitStudio v1.2 is the ability to edit the rules as you can in Designer; I haven't found a good way to edit rules yet. Besides that, and a few minor things, I think you'll be pleased with the functionality of CircuitStudio for its price tag. Note, if you're expecting to get exactly the schematic capture and PCB layout from Altium Designer when buying CircuitStudio you will be upset. It's very similar, but it's still different enough that I had about a 2 week learning curve as an intermediate Altium Designer user.



I applied for this RoadTest because of a conversation I had a few months ago. I asked someone if they had tried Altium CircuitStudio and their response was something along the lines of “If I’m going to use Altium, I’m going to use the real thing, not some crippled version”. I have used both Altium Designer and Altium CircuitStudio, and although I’ve noticed differences I don’t think CircuitStudio is crippled. Just for reference I have used the following tools in my career:


  • Eagle –. I’ve used it to design a power supply board.
  • gEDA – An open source schematic and PCB layout tool. I’ve used this to design a 4.6115 GHz PLL board.
  • KiCad – I tried to use this one, but got frustrated along the way.
  • Altium Designer – I’ve used this to design particle counter boards, Texas instruments booster packs, and daughter cards for development kits.
  • Altium CircuitStudio – I’ve used this to design a Semiconductor Optical Amplifier pulsing board.

Figure 1 shows a screenshot of the Thermo-electric cooler section of the PCB I designed using CircuitStudio. To be honest, I have been waiting for CircuitStudio for about 5 years. I’ve used Designer, and I find it overkill for my needs. I’ve only ever wanted schematic capture and PCB layout. At over $7,000 for Designer I’ve just found it too expensive for my needs. CircuitStudio costs about $1,000.



Figure 1: Snapshot of the TEC module for a board design.



The Interface

The first thing that will seem odd is this new ribbon style design. It’s very Microsoft like. I can’t say I’m a fan, but I’ve gotten used to it. Fortunately, a lot of the key commands are still preserved. Figure 2 shows the ribbon you would be presented with if you were in the schematic capture


Figure 2: Home Ribbon shown for Schematic Capture.


Laying out the schematic is very simple, just like Designer. The biggest change will be where you go to push your updates to the PCB. Figure 3 shows how to push the schematic changes to the PCB. It’s under the Home ribbon under the Project selection. I can almost guarantee you’ll forget where this is a few times. If you choose to use CircuitStudio, I suggest you make a physical note where this command is, because if you’re like me you’ll waste a lot of time looking for this one.



Figure 3: Pushing schematic changes to the PCB.


Part Creation

Most of the library functionality that you’d be familiar with in Designer is the same in CircuitStudio. The part creation wizard is available for the PCB libraries.  I never used the wizard, so I can’t comment on its similarity with Designers wizard. The one feature I miss considerably is the paste array function. This feature allows one to make a single pad with all the correct dimensions then simply copy and paste it in an array in either the X or Y direction with a given pitch. I’m hoping this feature comes back in version 1.3. Figure 4 shows the PCB footprint and schematic symbol of a BSZ15DC02KD device – a complementary transistor package.



Figure 4: PCB footprint and schematic symbol for BSZ15DC02KD.


As a short tutorial, let’s create a new part in CircuitStudio. If you’re not sure how to start a new project and create a schematic, I suggest you start with the beginner material Altium provides. Always check the vault to see if the part you want is there, or alternatively sometimes the vendors will provide the schematic symbol and PCB footprint on their website. Let’s create a part that usually doesn’t come with symbols or footprints. Let’s try the Thorlabs FPL1009S laser diode. Figure 5 shows the FPL1009S.

(Link to device:

The layout is given in the linked datasheet and in Figure 6.



Figure 5: 1550 nm laser diode in a 14-pin Butterfly package.



Figure 6: FPS1009S dimensions and pinout.



In CircuitStudio create a new schematic library -> right click the Projects area whitespace and choose Add New to Project -> Schematic Library. See Figure 7 for a screenshot showing the submenu and selection.



Figure 7: Creating a new schematic library.


Next, save the library by right clicking the newly create library and choosing Save As… from the menu that appears. Figure 8 shows this process. Then, select the SCH Library tab from the bottom of the Projects window. This is also shown in the bottom left of Figure 8.



Figure 8: Save the new library


Component_1 should appear in the pane on the left as shown in Figure 9. Click Add at the bottom of the pane and give it a name FPL1009S. Next, while FPL1009S is highlighted click Edit. The window in Figure 10 will appear. Change the default designator to U?, default comment to FPL1009S, and description to Laser Diode. Click OK to finish the changes. Note, the question mark for the default designator is intended. Altium uses the question mark when numbering parts in the schematic.



Figure 9 :SCH Library view showing Component_1



Figure 10: Edit properties for FPL1009S


Draw a rectangle using the rectangle tool highlighted in Figure 11. After drawing the rectangle, add pins to it. To add pins you can use the ribbon or right click the white space and choose Place > Pin. Once you’ve added the pins double click a pin to modify its display name and designator. When you’re finished, it will look something like Figure 13. Note, you can place a pin by simply hitting the p key as well.



Figure 11: The drawing tools for schematics.



Figure 12: Adding pins to the symbol.



Figure 13: Symbol after adding the pins.


To make the footprint, return to the Project pane and right click the project. Choose Add New to Project > PCB Library as shown in Figure 14. If you look at Figure 6 you might notice some information is missing. The vendor has not supplied the pin pitch. 14-pin Butterfly packages have a pitch of 2.5 mm.



Figure 14: Adding a PCB library (footprints)



Next choose the PCB Library tab from the bottom left corner of the screen. Right click in the Components white space and choose New Blank Component. Notice the option to use Component Wizard.



Figure 15: PCB footprint creation.


Double click the new component created and rename it to FPL1009S. For making the pads, you can use either the ribbon or right-click the working area and choose Place > Pad. See Figure 16 and Figure 17 for illustrations of the two options. Before you select a location hit the TAB key to get the options for the pad, or if you’ve already placed the pad double click it for the options menu shown in Figure 18.



Figure 16: Ribbon for Place options



Figure 17: Right click option for placing.


The default pad is a through-hole design, but the FPL1009S is a surface mount device. Change the hole size to 0 (mil or mm, whichever units you are working in). Next, make the X-Size 15 mm, Y-Size 1 mm, Shape rectangular, designator 1, Layer: Top Layer. The resulting pad should look like that of Figure 19. Just in case you didn’t center the pad on the drawing origin, make sure the X and Y location are both 0.



Figure 18: Options for Pad.



Figure 19: Surface mount pad for FPL1009S


Copy the pad by highlighting it (click it) and hit ctrl-c. You can also use the ribbon to copy if you wish. Altium will want an origin to copy from, so select the origin of the pad. The cursor should snap to the center of the pad when doing this. The next part would be easier if we had the paste array command, but we’ll just relocate the other pads manually. Paste the pad anywhere and double click it. In the window that opens change the X and Y location to 0 and -2.5mm respectively, change the designator to 2, and then hit Enter. Your display should resemble that of Figure 20


Figure 20: After adding the second pad.

Repeat this procedure for the next 5 pads. Your component should look like that in Figure 21. Next, we need to determine the x coordinates for the next row of pads. Per Figure 6 the width of the body is 12.7 mm. I’m going to design the body width in the footprint as 13.5 mm to give us a little wiggle room. This will allow for tolerances in making the PCB and in the packaging of the FPL1009S. Figure 22 shows the pads laid out such that there is 13.5 mm between them in the X direction.



Figure 21: Seven pads added to package



Figure 22: All 14 pins added to package.


In most instances, we would add lines to the Top Overlay layer to outline the package, but this style of package requires a board cutout. This is where it can get tricky because there is no direct way to do a cutout on the footprint. If you search, you will find lots of information on tricks to get cutouts in components, but it always comes back to the cutout occurring on the PCB and not as part of the footprint. I prefer to draw the cutout on the Top overlay of the footprint, then trace over it with the cutout tool on the PCB.

Note, the reference for the drawing is currently Pin 1. We’d like to move it to the center of our device. Go to the Home tab and click references > Center (Figure 23).



Figure 23: Moving the reference.


Draw a rectangle on the footprint from four line segments. Start by drawing a single line as in Figure 24. The exact length doesn’t matter, because we will edit it later. Double click the line, and the window of Figure 25 will open. Modify the line so that it starts at X: -256 mils, Y: 630 mils and ends at X: -256 mils, Y: -630 mils. The lines will begin and end at the four corners of the rectangle. The dimensions of the four corners are simple because we moved the origin to the center:

Upper left Corner is X: -256, Y: 630.

Lower left corner is X: -256, Y: -630

Lower right corner is X: 256, Y: -630

Upper right corner is X: 256, Y: 630

Units are all mils. Add the other three lines to finish the rectangle as in Figure 26.



Figure 24: Beginning the Top Layer drawing.



Figure 25: Editing a line segment using the dialog box.



Figure 26: Rectangle on footprint Top Layer


The next part to consider is the cutout for the fiber boot (the assembly coming from the laser). Some designers make a cutout for it and some don’t. I find it more flexible to add a section for the boot because it gives more flexibility with heat sinking the device. If I haven’t mentioned it yet, the reason there even needs to be a cutout is because the device needs to be bolted to a heat sink on its bottom side. A block of aluminum does a nice job. An example of a laser diode driver would be the PicoLAS BFS-VRM-03 shown in Figure 27. You can see the aluminum portion with the four mounting holes on the bottom side that act as the heat sink.



Figure 27: PicoLAS Laser Diode driver with built in heat sink.


Since different boots can be different sizes, let’s make a cutout that is 20 mm long and 7 mm wide. With the reference still at the center we will simply add another three lines and then trim the connecting parts. After all we’ve been through adding the lines should be straightforward, so I will not include the math to determine the line start and end values. When you’re done hopefully the result looks something like Figure 28.



Figure 28: Finished footprint.


Click File > Save All and the component will be saved. You can now add the schematic symbol to your project and then set its footprint to FPL1009S.

To get the cutout, you’ll have to trace around the layout with the Board Cutout tool on the Home tab of the PCB editor. If there is more interest after I post this review, I will consider taking the project further and show the PCB layout and board cutout tool. As for now, this RoadTest is over.



Some useful Hot Keys - In PCB editor (2D mode)

  • - Shift-s: This will mask the current layer selected. Basically, you can only see and select things on the current layer. It’s very helpful if you are selecting a few traces and changing some properties, since you may be presented with a list of possible choices from different layers if you click without the mask on.
  • - While routing hit TAB to edit the properties of the trace you are about to connect.
  • - While routing, SPACEBAR will flip the trace angle position.
  • - While routing hit SHIFT + SPACEBAR to toggle between trace styles. Very important for doing complex board cutouts.