The PCB Design Professionals

 

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.

 

 

 

Step 1

Download and install blender:

Blender

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.

 

Step 3

Download and install STLtoSTEP:

STLtoSTEP

 

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.

3D Content Central

 

We hope you found this useful and, as usual, if you would like us to cover a specific topic then please drop us an email.

 

Black Stick Ltd – Call the design line on +44 (0)1782683782

 

 

 

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.

 

Below is a short video showing the above steps.

 

 

 

PCB Layout Tips – DFM

Via Size

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.

Check out  our PCB Design page.

 

PCB Layout Tips – Ground Planes.

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.

 

PCB Layout Tips – Routing

 

Right Angle Tracks

Avoid right angle tracks where possible as they can cause issues with signal integrity. Also, on finer tracks they can cause the trace to be broken due to acid traps and erosion over time (see acid traps).

T – Junctions

It is advisable to avoid T junctions as they lead to impaired signal integrity. They can also cause acid traps on each side, which gives a higher chance of causing an open circuit.

Tracks from the board edge

The general rule for placing tracks from the board edge is three times the minimum track spacing I.e. track spacing 0.254mm(10 thou) then track to board edge should be at least 0.762mm(30 thou). But the bigger the distance the better.

Antenna

Antenna are small tracks that don’t join to another net causing and picking up noise.

Loops

It is best to avoid loops where possible as they can cause a large amount of noise, which in turn can affect the signal integrity of many tracks on your board. Also they cause inductance which can also lead to increased noise.

Acute Angles

Acute angles during the routing of a PCB can cause acid traps. This is where the etching solution gets trapped in the small corners and over time can etch away the track which can lead to an open circuit.

Track Spacings

The minimum track spacing is dependant on the voltage the tracks are carrying, this can be worked out in our C4 calculator . Generally if spacing goes below 0.127mm(5 thou), manufactring costs can increase.

If you need any help with your PCB layout we’d be happy to help check us out on our PCB Design page.

 

PCB Layout Tips

At Black Stick we would like to help engineers get started in PCB layout. We aim to do just that with this section and over time we’ll be posting about every aspect of PCB Layout from component creation to generating outputs.

 

If you would like to help this resource to grow please send your content to tips@blackstick.co.uk and we will add it into this page.