We have created this blog to try and engage and inform the electronics industry on how we do/see things here at Black Stick. We want to give the electronics community a better understanding of how things are viewed from a PCB Design point of view and hopefully, along the way, we will tell you things you didn’t know and make you question things you did.
We also have a guest bloggers area and are always looking for like minded companies or individuals who have a passion for the industry or have something to say.
Please feel free to get in touch for more information on Black Stick Ltd.
Black Stick are providing PCB Design training, using the Altium toolset, for Andrew Fielding who will be representing the UK in the Electronics category.
WorldSkills London 2011, the world’s largest international skills competition, takes
place from 5 to 8 October at ExCeL London. Team UK consists of 43 of the UK’s
most talented apprentices, employers and learners in 37 skills such as electronics,
mobile robotics.
This post was brought about by another of our customers needing the ability to create detailed STEP files for their components. Usualy this would entail buying solidworks or something similar.
We knew that we could do it cheAper, and with 3D PCB Design becoming ever more important, we thought we’d share this with the PCB Design community.
Altiums built in 3D extrusion tools are great (and getting better all the time). We expect to see some pretty big jumps in what you can do within Altium in the future. Until that time, try the steps below.
Blender is not a point and click program, so you will need to spend a bit of time getting used to the user interface. However it is free (open source) and worth the effort of learning, as it’s extremely powerful.
Step 2
Once you have the hang of blender and have created your model (or alternatively you can add one of the standard meshes to try it out).
Now export your model from blender as a .obj or .stl. We have found .obj gives better results.
You now have your model ready for converting to a STEP file.
This programe allows you to convert 3D models from STL (or OBJ) to STEP. This little gem is the key to getting your models into Altium.
Allthough this is a free programe, the developers request that if you use it commercialy then they would appreciate a donation (which is fair).
Step 4
From STLtoSTEP select File>Open OBJ
Browse to and select your recently exported obj model (This may take a while depending on the complexity of your model).
Now select File>Save STEP (FACETS).
Your Step file is now ready to import into Altium.
Step 5
Read your models into Altium.
Your done!
Below is a short video showing the above steps.
It’s worth noting that 3D Content Central have quite a nice selection of ready made Step files for a large variety of components. Have a look, it might save you a bit of time.
One of our customers needed the ability to import just a drill file into Altium and asked if we could help. Getting Gerbers into Altium is easy enough, but just the drill file was posing a problem.
The following instructions (thanks to the Wonderfuly Spectacular Jo for the lovely walkthrough) give a step by step guide on how to import Microwave office files and a drill file into Altium.
Importing Microwave Office files and adding drill data
1. Export microwave office job as a PADS file
Open Microwave office project (file extension EMP)
Options >Drawing Layers
File>Export Mappings (RMB) New PADS file Export Mapping
Layout>Export>Save as Type>PADS *.asc
2. Export microwave office drill file
Layout>Export>Save as Type>NC Drill *.txt
NOTE:
Because Microwave office does not create a netslist, it is not possible to translate directly into a PCB, so interim steps have to be taken in CAMtastic to create a netslist first.
This is done by creating two dummy gerber layers, copying the shapes from the drill file onto these layers and assigning them a Dcode. By having these dummy pads and a drill file tying them together, it enables a netlist to be produced and the file exported to PCB.
3. Import PADS file into Altium
File>Import Wizard>PADS ASCII Design and Library Files
Fill the search path for the PADS job you have exported. Ignore the library. ‘Next’ to everything…
A new PCB file will be created. Move into the appropriate project area.
4. Import drill files
Open CAMTASTIC. File>New>CAM Document
Import drill data. File>Import>Drill
Navigate to directory and import .txt file
Settings to be 3,3 Absolute and Trailing
5. Add two layers
Using File>Layers>Add, create two layers called top.gtl and bot.gbl (file extension names are critical to ensure they are assigned the correct layer in CAMtastic)
Assign these new layers to the correct PHYSICAL layer.
Tables>Layer Order. In the Physical Order box, assign .gtl to layer 1 and .gbl to layer 2.
6. Copy drill holes onto the top and bottom copper layers
Edit>Layers>Copy to Layers. Select all shapes on the drill layer. RMB to bring up new menu. Select the top and bottom layers that you want the shapes copied to.
7. Create a new Dcode
Using Tables>Apertures create a new Dcode. Suggest using D10 and assign a pad size suitable for the drill size in the job.
8. Assign Dcode to the holes on top and bottom layers
Turn off drill and bottom layers. On just the top layer:
Edit>Objects>Modify/change. Select all shapes on the top layer. RMB to bring up new menu. Select Use Dcode 10.
Repeat for the bottom layer.
You now have a drill file and two gerber layers. The drill holes correspond to pads created on the gerber layers.
9. Extract a netslist and export to a PCB
Tools>Netslist>Extract
File>Export>Export to PCB. This will create a new PCB. You can now cut and paste these into the PCB created from the Microwave office job and modify as you wish…
Using PCB inspector the pads can be deleted or modified and the nets can be changed to ‘NoNet’ to remove net name assignment.
As a general rule for standard via’s, the pad should have at 0.15mm(6 thou) annular ring (e.g. finished hole size of 0.3mm(12 thou), pad size of 0.6mm(24 thou)). This provides a tolerance for drill wander to avoid drill breakout.
Via Tenting
Tenting your via’s (i.e flooding them with solder mask) reduces the chances of a short from adjacent exposed pads. It all so allows you to place your silk screen designators over the top of via’s without part of it disappearing down the hole and becoming illegible.
Via to Pad
Try to keep vias at least 0.15mm(6 thou) away from pads as if they get too close then untented can steal the solder from the component pad or could cause tomb-stoning issues. If this is not possible try tenting the via’s as above.
Silkscreen rules
Silkscreen should be kept between 0.10 mm(4 thou) and 0.20 mm(8 thou) away from anything conductive that’s not covered by solder mask. The minimum line thickness should be 0.15mm(6 thou) and the minimum letter height should be 1.0 mm(40thou).
Fiducials
Adding fiducials is a must for any board which uses surface mount components. These little copper islands give the pick and place machine an accurate triangulation point (you’ll need a minimum of three fiducials per side) which will help to get your components placed accurately and also makes sure that the board is orientated correctly before placement starts.
Hole Size
The hole’s in your board (whether for component legs, mounting hole’s or via’s) need to be drilled. Generally the smallest standard drilling hole size a manufacturer can drill is around 0.2mm(8thou), any smaller than this and they will more than likely need to be laser drilled micro via’s which can be very expensive.
Track Width
While there is no definite bottom line for track width, if you’re going to be using less than 0.2mm(8 thou) you may want to contact your manufacturer and ask them what they are comfortable going down to. Most manufacturers will happily etch 0.127mm(5 thou), but you don’t want to find out they can’t after you’ve routed your board.
The above are rough guidelines, and your design, fabricator or assembly house may have different requirements abilities.
If you need any help with your PCB layout we’d be happy to help.
Power and Grounding is one of the first things you should consider when planning your PCB layout. Good grounding is essential in minimising potential EMC problems with your finished design. We have outlined some basic things to think about when laying out your design.
2 Layer Boards.
The best construction for a two layer board is tracks on the component side of the board and a full ground plane on the oposite side. Being realistic though, a board with single sided tracking is not always an option. In this situation we would add a ground plane to the component side and “stitch” this together with vias. When using this approach, try to place your tracking over solid sections of ground plane and not cross any breaks in the plane. Crossing a break in the plane increases the length of the return path of the signal which in turn increases the chances of having EMC problems.
If your ground plane gets really broken up consider changing to a four layer or more board construction.
4 Layer or more boards.
Even with 4 or more layers and a solid ground plane or two, you can still run into problems we’ve listed a few things to look out for.
Mixed Grounds.
If you have seperate analogue and digital ground, try to keep their planes completely separate in their own little section of the board. No digital tracks should cross into the analogue plane area and vice versa. Also if you have a corresponding analogue power then try to mirror the power plane on an adjacent layer.
General Things to Consider.
Direct Connect Via’s – Unless your going to solder something into a via, there’s no need to thermally relieve them. Direct connecting vias to planes helps to provide a plane with less gaps.
Pull planes back from the board edge – Keeping your planes away from the board edge can help to reduce the chances of your power and ground planes edge coupling. Also, if your planes are exposed during the routing process there is the chance that your power plane could short to the case or even your between internal planes. The pullback distance should be at lease 3 times your minimum gap, but allow more if you have the space.
If you need any help with your ground or power planes we’d be happy to help. Check us out on our PCB Design page.
The days of throwing the schematic over the wall to the PCB guy were over a long long time ago. Letting the PCB Layout Engineer know about the sensitive tracks on your design, whether it’s impedance tracks, High Voltage, High Current, and (increasingly) Low Voltage etc, can mean the difference between a successful layout, or being left with a pile of scrap . In this post we are going to try and give you a few ways to add things to your schematic that can help in conveying this critical information.
Directives
A useful way to pass information from the Schematic to the PCB are directives. They can be found in “Place” —> “Directive” or by typing P V in an active schematic window. The advantages of directives are that they are easily seen in the schematic and they pass information into the PCB Layout which can be shown in the PCB Panel (The PCB Panel will be covered in post 17). You can also add rules to the directive to constrain the attributes of the tracking; width, clearance, maximum via count, basically all the rules that you can normally set in the PCB domain, can be assigned using directives.
We recommend not to constrain the PCB Layout Engineer too much by inflicting tight rules. For example: If you have a 40 Amp track and you set a minimum track width of 7mm. It is very hard to get a 7mm track out of a decoupling cap pin. The designer may have to split the track many ways to achieve the required width and if you have a rule fixing this nets width at 7mm he won’t be able achieve this (it’s better to have a 40Amp net class).
Let’s start with the “Net Class”. Iif you want to show a high current, high voltage or single ended impedance line, a net class directive is one way you could do it. Place a Net Class Directive with “Place” —> “Directive” —> “Net Class” or P V C, you’ll then find one attached to your cursor and you can place this on any net line. Once placed double click the Net Class and give it a name (You’ll need to do this in the name box and the class name attribute). You can now copy then paste and put the net class where ever you need one. If you want to differentiate a net class just change the name and class name attributes and they’ll appear as separate entries in the PCB.
A “Blanket” is a way to capture areas of circuitry. Rather than adding a net class to each net, you can draw a blanket as (shown on the right). To draw a blanket got to “Place” —> “Directive” —> “Blanket” or P V L, draw a box around your Schematic Symbols. You can now attache a Net Class or other directive to this blanket.
No ECR is a red cross that can be put on items that will stop Altium from including them in the Rules Check (Dangerous so BE CAREFUL). One way to use this is to place it onto pins that are intentionally left unconnected. This not only lets the PCB Layout Engineer know that the single pin net is acceptable, but also lets Altium know, and you should see less errors in your Schematic Compile.
We hope these have helped. If you would like any further information please feel free to post up a comment.
Hi I’m Dong Nong, Design & Test Engineer at Ohmega Technologies, Inc and I’d like to give an introduction into what OhmegaPly ® is and how it can be used in your PCB Design.
OhmegaPly® is a Nickel Phosphorous (NiP) metal alloy that is electrodeposited onto the matte, or tooth side, of copper foil. The thin film NiP metal alloy/copper foil combination is called OhmegaPly® RCM (RESISTOR-CONDUCTOR MATERIAL). The RCM is laminated to a dielectric material (like any other copper foil) and subtractively processed to produce copper circuitry and planar resistors.
Now you know what OhmegaPly® is, why should you use it in your design.
Because of its thin film nature, it can be embedded within layers without increasing the thickness of the board or occupying any board surface area as is required for discrete chip resistors. Allowing you to reduce passive component density and increase active component density leading to reduced board form factors. By placing your resistors inside the board you also reduce the number of vias meaning more room for tracking. There are electrical, economic and reliability advantages of using OhmegaPly® you can find out more about these by visiting our Technology Page.
Black Stick would like to thank you for your support and custom over the last year and wish you a very happy and fruitful 2011.
We started our blog around this time last year and we have tried to engage the electronics community with a view to giving a better understanding of PCB Design and how we integrate with other areas of the electronics industry. We are starting to see some results in this area as we have some guest bloggers working away on unique content. Which we hope to have the first of live shortly.
We have seen a dramatic increase in visitors and we are now seeing over 700 visitors per month. Our Altium post are proving popular and we will continue to post these as often as time allows. Also with the imminent release of Altium Designer 10, we will cover the main changes and improvements in the software that affect PCB Design.
As always if there are any topic you would like us to cover please post up a comment or drop us an email blog@blackstick.co.uk
Altium Designer 10 is due for release on the 31st of January 2011 there are lots of new features that you can find out about on the Altium Release 10 website.
Contact Us
Sitemap
home
