The PCB Design Professionals

What’s coming in Altium Designer Release 10

We’ve been looking into the up-comming release of Altium Release 10 and the most exciting features being a PCB Layout company are the Enhanced routing capabilities and Structured classes in PCB editor.

Enhanced routing capabilities

The routing engine looks as though it has been improved to include multi-routing with 45 and 90 degree corners and arcs. Loop removal has also been extended to apply when tracking multiple tracks.

Structured classes in PCB editor.

Structured classes should allow you to create hierarchical classes from the schematic they are then viewable in the PCB editor. You should then be able apply rules to the classes in the design rules panel.

Some of the other features included in Release 10.

• Smart Data Management.

• Peripheral Register View.

• Atmel Qtouch(R) Support.

• 3D PCB ‘flyovers’.

• Variants Shown in PCB editor.

• 2G/3G Mobile connectivity enhancements.

• USB wifi support.

• Aldec OEM simulator.

For more information on Altium Release 10 follow this link – Release 10

Power Planes – 11 Part 2

So continuing from where we left off I guess we better talk about positive planes.

Positive Planes

So far we have drawn our negative plane and added a split to it, after all that hard work you’ll probably want to switch it off now to make it easier to see the positive plane. You can do this by going to “Design” then “Board Layers & Colours” or hit “L” for short, then there is a internal planes column in the middle you can un-check the tick box to hide our internal plane.

Now we can see what we are doing you can add a polygon pour (positive plane) by going to “Place” then “Polygon Pour” or hit “P” then “G” you will be presented with a dialogue box like this.

In here there are a number of different options (I’ll let you discover most of them). The basic ones are Name, Layer, and Connect to Net. Name is just an identifier (can be a life saver on boards with many polygons), layer is fairly straightforward the layer you would like your polygon to be on and Connect to net is also an easy one the net you would like to connect with your polygon. If you set all of these things and press OK.

You should now have a cursor on the end of your mouse that you can use draw your polygon any shape you like. The polygon draw tool is much the same as the tracking tool in that you can press shift and space to change the line style between – Right Angle, Any Angle, 45, Arcs and curves. with a combination of these you can draw a fairly complex shape.

If you would like to edit the polygon after placed you need to right click on it go to polygon actions then move vertices’s this will give you a number of pick point to modify the corners. If you want to stretch a certain section you need to click the line in between the pick points.

Polygon pours do not automatically re-pour so should you need to re pour your polygon you can either double click on it to bring up the dialogue box then click OK to close it you will then get the option to re-pour your polygon. You can also right click and as before go to polygon actions but this time go to re-pour this will re-pour the polygon you right clicked on. There is also the Tools menu, go to “Tool” then “Polygon Pours”  there are few re-pour options there. Then there is the Polygon Manager but we’ll cover that in another post.

What else do you need to know about polygon pours -

One fairly important one I should probably mention is that if you draw a smaller polygon inside a larger one, two things will happen.

1. The clearance between the two will be your minimum whole board clearance unless you set another rule specifically for the polygons.

2. Depending on the order you draw the polygons in the larger poly may pour right over the smaller. To avoid this you will have to use the Polygon Manager to set the pour order (auto generate usually works out fine).

Pros

• Can be use on layers with tracks.
• Dead copper can be removed.
• Easily understandable (WSYWIG).

Cons

• Sometime slow to re-pour.
• Does not auto generate.
• Can take up quite a bit of system resource.

Well I hope that’s given you a start into power planes in Altium if you have any questions or you would like us to do a tips and tricks on a specific topic, post a comment or email us at blog@blackstick.co.uk

Power Planes – 11 – Part 1

There are two ways to set up your power planes in Altium either a positive plane or a negative plane. Each have their pros and con’s and I’ll try and touch on that as we explain both.

Firstly we will need to add some extra layers to the design  to do this go to “Design” and then “Layer Stack Manager” or hit “D” then “K” for short. You should get this dialogue box.

I’m going to use a 4 layer design for this example, so I need to add a power plane layer and a normal internal layer for our positive plane. All you have to do is hit the Add Plane button on the right hand side and the add layer button, and you should end up with something like this.

So now you have your four layers one for the negative plane you will also need to define the Net that will exist on that layer. If you double click the Internal Plane layer ((No Net)) you should get a dialogue box that allows you to change the layer name, copper thickness, net name and plane pullback, select your net and click OK. Click OK again to close the Layer Stack Manager.

Negative Planes

OK so we have pretty much set up our negative plane in the layer stack manager but the are a few things you can change.The pull back from the board edge in layer stack manager if required. Also if you would like to split a negative plane layer so that it has more than one net on it this is possible by drawing a line on the plane layer. The thickness of the line determines the clearance between the two planes (pictures Below).

Well thats about it for the basics of negative planes, have an play and see how you get on. I’ve listed a few pros’s and cons below as promised.

Pros -

• They automatically update
• Are fast to redraw
• Take up minimal system resource.

Cons -

• You cannot draw tracks on a negative plane.
• There is no way to remove dead copper from a negative plane
• They are not as easy to understand as a positive plane.

Part 2 will cover how to draw and manage positive planes keep your eyes peeled. If you have any questions or you would like us to do a tips and tricks on a specific topic, post a comment or email us at blog@blackstick.co.uk

PCB Inspector – 10

OK so I briefly mentioned the PCB Inspector in the find similar Find Similar post, I’ll go on now to talk about some of the things that we use the inspector for.

I should probably describe the basics of the PCB Inspector itself there are two main elements;

• The first is the include only option it’s the blue link text located just under the title bar. With this you can filter your selections to include just the items you want, e.g. Tracks and Arcs but not Vias and Pads. You can also get it to display all selected objects.

• The second area which is basically everything under the “Include only” text is the editable parameters of your selection.

OK so what can you use the PCB Inspector for?

Changing Track Widths.

Changing track width globally or local is quick and easy with the PCB inspector. Select your tracks (you can use “CTRL + H and “Find Similar” to make this quicker) then under graphical, change the width. One thing to be careful with is that if you have arcs in your track you will have to make sure that arcs are listed in the “Include only” section.

Changing Ref Des Size / Position.

If you want to globally change the size of your component references then Find Similar and the Inspector are your friends here. First select all you references using Find Similar then in your PCB Inspector you can firstly change the size by altering the text height and width under graphical and secondly you can auto position the references by adjusting the auto-position drop down box.

Those are just a few of the things that the PCB Inspector can be helpful for. Basically if you want to edit a group of objects then it will probably be the best tool for the job.

If you have any questions or you would like us to do a tips and tricks on a specific topic, post a comment or email us at blog@blackstick.co.uk

3D Component Design – 09

So now you can view your PCB in 3D you probably want to add some 3D information to your components.

I’m going to use a surface mount cap for this example. The first thing you want to do is draw the outline of the body in 2D on a mechanical layer (Image 1). Then if you go to “Place” then “3D Body” or press “P” then “B” you should get a dialog box where you can enter the 3D information (Image 2).

In this example you’ll want to choose extruded from the 3D model type box. After that set your mechanical layer, heights and colour click ok to draw your 3D shape. Now if you have your electrical grid turned on and your active layer is the mechanical layer that you drew the 2D outline on then your cursor will snap to the corners of your 2D shape. Click on each corner to define your 3D shape right click to finish. The 3D dialog box will pop up again you can just close this (unless you want to draw another 3D shape).

Now if you press 3 you can view your newly created component in 3D and it should look something like image 3. With a bit of patience you can create some quite nifty components, here’s one I made earlier shown in Image 4.

If you want to make some really detailed and accurate components you can model them in a 3D package, then, import a step file straight into you PCB library.

Enjoy making 3D components, if you have any questions or you would like us to do a tips and tricks on a specific topic, post a comment or email us at blog@blackstick.co.uk

3D – 08

Viewing your PCB in 3D in Altium is as easy as, well… 1 2 “3″. All you have to do is press the number “3″ or go to “View” then Switch “To 3D”. To return back to 2D (you guessed it) press “2″.

Once you have your 3D view you will probably want to zoom around the components pretending you can fly.

To Move in 3D you can:

Zoom: Press both mouse buttons together and move the mouse forward and back, or hold “CTRL” and use the scroll wheel on the mouse.

Pan: Scroll wheel pans along the the X axis and “SHIFT+Scroll Wheel” and along the Y axis. (Hold down the right mouse button to drag the screen with the hand tool).

Hold down the shift key to show the navigation ball, (shown in “Image 3″)  then you can right click anywhere on the screen to rotate your PCB on all axis. The navigation ball also has four arrows and a circle. Right clicking on any of these will allow you to lock the rotation to that axis only.

Press “V” to bring up the view options where there are a number of different choices. A few of the really handy ones are “V” then “B” this flips the board, “0″ (Zero) will return your view to 0 degrees, Pressing “9″ will change the view to 90 degrees and finally press “2″ to go back into 2D mode.

So that was viewing your PCB in 3D, the next post will be about defining the 3D attributes for your components.

If you have any questions or you would like us to do a tips and tricks on a specific topic, post a comment or email us at blog@blackstick.co.uk

Tracking – 07

I guess we should start with how to place a track you can either go to “Place” then “Interactive Routing” or click the interactive routing button or press the shortcut keys “P” then “T”.

Now you’ve got your track on the end of your cursor what can you do with it?

• Changing the track segment – “Space-bar” flips the direction of the corner of the track.

• Toggle the tracking mode – “Shift + Space-bar” 45 Corners –> 45 Arc Corners –> 90 Corners –> 90 Arc Corners –> Any Angle tracking.

• Placing the tracking – Click the Left mouse button or enter to place the segment.

• Adding a via – Press 2 to add a via, or hold shift while scrolling the mouse wheel to toggle between electrical layers you can also use “+” and “-” to change layers.

• Cancel your tracking – either press escape or right click.

Ok so now you have some track on your PCB how do you edit it well. There’s a number of different ways of selecting and editing the tracks you can:

• Left Click to select the track and then Left Click and drag the corners or center of the track to edit that segment.

• Left Click to select the track and then Left Click and drag anywhere except the corners or center of the track to stretch that segment.

• Double click to change the tracks segment properties width, start end co-ordinates etc. To change the whole track you can you “CTRL + H” (select connected copper) then use the PCB inspector to alter the track.

• If you have multiple tracks selected you can track them all at once by clicking the Interactive Multi-Routing button or from the menu “Place” then “Interactive Multi-Routing” or press “P” then “M” for short.

There’s also interactive length tuning but that’s a whole other post.

As always if you have any questions or you would like us to do a tips and tricks on a specific topic, post a comment or email us at blog@blackstick.co.uk

Find Similar – 06

Find similar is another really handy tool for making global edits to primitives. All you have to do is “Right Click” on the object you would like to find more of or edit and choose “Find Similar” from the pop up menu. Alternately you can go to “Edit” then “Find Similar” or press “E” then  “N” or “SHIFT+F”. You will then be presented with a dialogue box as pictured.

From here you can tighten your parameters and make sure you select just the thing you are after. Also at the bottom there are option for how your results will be viewed and also has a run inspector check box which if checked will pop up the PCB Inspector window so you can make your edits straight away.

If you have any questions or you would like us to do a tips and tricks on a specific topic, post a comment or email us at blog@blackstick.co.uk

Rules – 05

Design -> Rules (D R)

The design rules in Altium are very powerful and it would take us an age to type an in depth blog on the rules. So here are a few of the one’s we use.

Polygon Rules

You have to keep an eye on polygon rules  if you use the query helper and select polygon from the object types checks, then the syntax would be ‘ispoly’ we have found that this doesn’t work, instead you can use the syntax ‘inpoly’ to set up rules for clearance checks or direct connects to polygons.

Unused BGA pins Rule

If you have a BGA with unused pins that you still want to fanout to a via. You will get short circuit error between the ‘no net’ pad and ‘no net’ via and track. There is away around that though, you can add another short circuit rule to be as pictured. This should fix those ‘no net’ errors and stop any other short circuits.

Tenting Via’s

Tenting via’s is a neat  little rule and pretty simple too. The rule is under the Mask heading, then Solder Mask Expansion. The syntax for a via is ‘isvia’, the rule is structured as pictured. Just make sure the expansion value is set to at least the minus of your via pad size. (eg. if your via has a 24thou pad then your expansion rule should be -12thou).

Clearance area’s

If you want to set up a specific area on a board to have a smaller clearances than the rest of the board (say for a fine pitch BGA) but you don’t want to extend this clearance over the whole board.  You can use a room  that has been pulled in from the schematic or create a new one from scratch. You can then create a rule similar to the one pictured.

If you would like us to list a rule that’s giving you trouble let us know – blog@blackstick.co.uk

Convert – 04

The convert command is great for creating unusual shaped copper pours or board cut-outs. It is located under the Tools Menu, Tools → Convert or type T then V. for short. I’ll put the short cut keys in brackets from now on.

Say you wanted to create a circular board cut-out you could use.

- Design → Board Shape → Define Board Cut-out (D S C) It’s is hard to draw a circle of an exact size and shape.

Instead draw a circle using Place → Full Circle (P U) which allows you to define a circle with an exact radius.

To make this a board cut-out (you guessed it). You can use the convert tool, Tools → Convert → Create Cut-out From Selected Primitives (T V B).

Similarly you can do this  for a complicated copper pour area or even convert to a region to make a keep out area on any layer.

The convert tool really comes into it’s own when working along side a mechanical engineer, you can import mechanical drawings lets say for example a metal can that touches the board in several places. You can convert this drawing into a keep out and banish tracks components and via’s in that area forever.

If you have any questions or you would like us to do a tips and tricks on a specific topic, post a comment or email us at blog@blackstick.co.uk