PCB Design News
Creating and importing Step files into Altium for free
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 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:
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.
Importing Microwave Office files and adding drill data Into Altium
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.
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.
Altium Designer Help and Tips - Schematic Directives
Schematic Directives
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.
Altium Designer Help and Tips - Output File Settings
Output File Settings
Following on from the Output Job files post, here is how to set up the output files.
ODB++
Is fairly simple to set up double click on the output file you will then have the ODB++ setup box in front of you. On the left hand side you have the layers to include in your output. Check the text boxes for the layers you would like to export. Check the right hand box if you want any layers to include on all layers, alignment marks and drawing frames etc.
All that is left to set up now is the board out line layer in the drop down box in the bottom right. Press OK and the ODB++ files have been set up.
Gerber Files
The Gerber files setup is slightly more complex, there are a number of tabs which I’ll explain below:
General – In the general tab you can choose your units and the format of the gerbers which is the precision your gerbers will be.
Layers – This tab is very similar to the ODB++ setup as in you have to check the layers you would like to out put and also check any layers you would like to see on all layers.
Drill Drawing – Here you can set the drill drawing and drill guide plots check the box to enable them, then choose how you would like the drill drawing drills to be represented on the right hand side.
Apertures – The only option you should need to check in here is “Embedded apertures (RS274x)” It is enabled by default but it’s worth a check to make sure.
Advanced – Film size is of interest here. Some times you may get a “film size too small” error when you run your gerbers. The “Film Size” area of the advanced tab is where to fix it by increasing the x and y size and possibly decreasing the border size if you reach the maximum extents of the film size.
Pick and Place Files
Probably the easiest output to set up. Double click “generate pick and place file” then pick your format “CSV” or “Text” (we tend to output both as then the assembler can choose which he’d prefer). Then set your units. Easy!
Bill of Materials (BOM)
Ok, there are 4 main areas in the BOM set-up dialogue box; “Grouped Columns”, “All Columns”, “Export Options” and the largest the bom preview window.
Firstly you’ll probably want to select you headings, this can be done by checking the boxes in the “All Columns” area. Doing this will add your headers and information into the preview area.
So you’ve added your headers, what next? You may way to group the rows by type (comment, footprint etc). You can do this by dragging the item from the “All Columns” section into the grouped columns section and then checking the box next to it.
You can also order your heading by dragging them to the left or right in the preview area. This will allow you to get a bom to export in your preferred format.
So that leaves us with export options there are a few to choose from and I’ll let you experiment with each in your own time. The only thing I would mention is if you are using a database Library be sure to tick the “Include Parameters From Database” check box or you may miss some information from the BOM.
Altium Designer Help and Tips - Output Job Files
Output Job Files
So you have a finished PCB layout, and you want to get your PCB fabricated. This post should hopefully point you in the right direction to getting your PCB’s output and off to be made.
Adding an Output Job File
Firstly you’ll want to add an output job file to your project “File” – “New” – “Output Job File” you should then be presented with an Output Job File with a lot of different outputs that are all configurable. Don’t worry about all the choice – there are only a few that need to be outputs for board fabrication and assembly purposes.
The PCB fabricators will need:
“ODB++” or if they don’t accept ODB++ then “Gerber Files” and “NC Drill Files”
The PCB Assemblers may thank you for:
A Pick and Place File and a Bill of Materials.
This is the minimum to allow you to get your PCB Layout manufactured. I’ll talk about how to set up these files in a subsequent post.
You’ll need to set what kind of outputs you want and where you want them to be stored, luckily I’m going to explain how to do just that.
Choosing the output type.
Click on the output type you want (for example PDF – shown opposite) then click the radial button for every output file you would like to be generated as a PDF. The greyed out boxes cannot be output as PDF i.e Gerber files cannot be output as PDF’s for obvious reasons. You can then repeat this for the other output types. If your output type not listed (network printer etc) then click “[Add New Output Medium]” and select the desired output from the list.
Choosing where your outputs are stored.
To do this right click on the output and click PDF Setup in the case of PDF’s, similarly Generated File Setup for Generated files and so on. In this window you’ll be able to choose your save location and file name here as well as a many other options.
All that’s left to do now is click your output and then click the Publish to PDF button at the top or press F9.
Altium Designer Help and Tips - Custom Board Shapes
Creating Custom Board Shapes
There are two main ways we use to create board shapes they are by Creating a Shape or importing it from a DXF or DWG.
Creating a Shape.
Creating a board shape is quite similar to creating a cut out – Convert.
The first thing that you will need to do is draw a shape in primitives (tracks, arcs, etc) that represent your board outline.
Once you have the shape you need to select the primitives then go to “Design” -> “Board Shape” -> “Define From Selected Objects” once you’ve clicked this your board shape should change to the shape you have drawn.
Importing a DXF/DWG.
You can also define a board shape from an imported DXF. To import a DXF go to “File” -> “Import” DXF/DWG are the defaults but there other import options there. Navigate to your DXF or DWG file and open it. You should be presented with a dialogue box like this.
You’ll need to change a few settings as listed below.
Blocks – We usually check the “Import as Primitives” in the “Blocks” section. Importing as primitives is more flexible for editing at a later stage.
Scale – Set the scale to match that of your DXF/DWG. You get a rough idea of the size along the bottom of the “Scale” section.
Drawing Space – We usually select “Model” so that we don’t import any drawing borders and just get the relevant information.
Default Line Width – Fairly self explanatory select the line width for you imported primitives.
Locate AutoCAD (0,0) at – Use this to set the origin of your imported primitives. Either type the X and Y locations or click select and click again in the Altium Design Space to set the origin.
Layer Mappings – Use this section to set which layers of your CAD drawing import into Altium and on which layers.
Once you have all of these set up the way you want them, click ok and vew the lovely imported CAD drawing. Should you get an error message, or nothing imports, the most common cause we have found is that the scale has been set incorrectly and the import is too large for Altiums design space.
OK, so now you have your DXF imported it’s just a case of selecting the relevant sections of the Imported primitives and creating your board shape from selected primitives as above.
Altium Designer Help and Tips - Cross Probing
Cross Probing
Two ways we find helpful to see where things on the Schematic are on the PCB and vica versa, are “Cross Probe” and “Cross Select Mode”.
We’ll start with “Cross Probe”
To use it go to the Tools menu then “Cross Probe” you can also click on the “Cross Probe” button on the toolbar (we call it the stick of dynamite but I think it’s supposed to be a probe).
It may take a few moments for the selection cross hairs to appear, once they appear click on the component while holding down “CNTRL” and the components should pop up on screen. If you don’t hold control it will flash up and then return to your current document.
However if you are lucky enough to have two screens, an effective way to cross probe is to open the Schematic sheets on one screen and the PCB on the other. Doing it this way will allow you to easily highlight many components in a row without juggling documents constantly.
Next up “Cross Select Mode”
To use “Cross Select Mode” it has to be activated in both the PCB and Schematic. To do this go to “Tools” then click “Cross Select Mode”. You can now select groups of components in the PCB or schematic and see them high-lighted in the other environment. Great for checking proximity of your critical components.
Altium Designer Help and Tips - Power Planes Part 2
Power Planes - Part 2
So, continuing from where we left off, 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.
Altium Designer Help and Tips - Power Planes Part 1
Power Planes - 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 a play and see how you get on. I’ve listed a few pros 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.
Altium Designer Help and Tips - PCB Inspector
PCB Inspector
Before we get started i will 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.
Altium Designer Help and Tips - 3D Component Design
3D Component Design
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.
Altium Designer Help and Tips - 3D PCB Design
3D PCB Design
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.
Altium Designer Help and Tips - Routing
Routing
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.
Altium Designer Help and Tips - Find Similar
Find Similar
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.
Altium Designer Help and Tips - Design Rule
Design Rules
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.
Altium Designer Help and Tips - Convert
Convert
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.
Altium Designer Help and Tips - Short-cut Keys
Learning the shortcut keys is one of the ways to get the best out of Altium Designer.
If you look at the menu bar along the top the menus have an underlined letter (File for example). You do not have to move the mouse all the way to the top right just press “F” when the design area is active and up pops the file menu. Similarly most of the options within here have underlines to. So if you wanted to open up an new file all you have to type is “F O”. Here is a list of some of the one’s we use day to day.
Measuring
- R M - report measure (allows you to measure the distance between two points.) you can also use CTRL+M.
- R P - report measure primitives (allows you to get an edge to edge measurement of most design items).
Place
- P V - place via.
- P T - place track.
- P M - place multiple traces (allows routing of multiple traces i.e busses).
- P F - place differential pair.
- T O R - tools ? options ? room (allows you to place selected components in a room).
- T O L - tools ? options ? rectangle(draw a boxed area and components will be placed inside).
Selections
- S L - select touching line (draw a line and every thing touching that line will be selected).
- S I – select inside (draw a box and everything completely encompassed in the box will be selected).
- S O – select outside (draw a box and everything outside the box will be selected).
- SU – select touching rectangle. (draw a rectangle and every thing touching that rectangle will be selected.)
Aligning
- A L - align left.
- A R - align right.
- A C - align horizontal center.
- A V - align vertical center.
- A T - align top.
- A B - align bottom.
Origin
- E O S - edit origin set.
- E O R – edit origin reset.
Layers
- L - brings up layer tab in view configuration.
- CTRL+D - brings up”show/hide” tab in view configuration.
- SHIFT+S - toggle between single layer mode. (Hide, Gray Scale, or Monochrome other layers).
Nets
- N – brings up “show/hide connections” options for hiding net lines and of course making them visible again.
There are lots of short-cut keys in Altium and they are extremely useful once you get to know a few. Hope this helps.
Altium Designer Help and Tips - Moving components
Do you have a component on your cursor and don’t know what to do with it? Hopefully this post will help.
There are two ways to move a part in Altium you can either click on the component and then drag it, or click the component and click the move selected objects button (which allows you to move the parts by a specific point).
Schematic & PCB
- Arrow Keys - Moves cursor 1 grid.
- Shift + Arrow Keys - Move cursor 10x grid.
- Spacebar – rotates components clockwise.
- Shift+Spacebar - rotates components anticlockwise.
- X - flips components on the X axis.
- Y - rotated components on the Y axis.
- TAB - bring up all the component information.
Just PCB
- L - toggles the layer that the component is on (top side/bottom side).
- CTRL+G allows you to change the placement grid for the component you have attached to your cursor.
- CTRL+D snaps components to the placement grid.
- TAB - Then change the x/y co-ordinates to where you would like the component to be.
***Warning do not use X or Y when placing a component in PCB Editor or your component footprint will be mirrored***
Altium Designer Help and Tips - Altium Environment
Altium Environment
Design Space Layout
Design space layout in Altium are completely isable you can move the majority of the windows where you would like them to be. There are some defaults set so if you misplace a window then View —> Desktop Layouts is your friend.
Zooming
-
Hold the middle mouse button and move the mouse forward and back.
-
CTRL+ scroll wheel.
-
CTRL+ hold down right mouse button.
-
Page Up – zoom in.
-
Page Down -zoom out.
-
Right Click then Left Click then move in and out.
Moving
-
Hold the right mouse button to grab the screen
-
Mouse scroll wheel pan up and down
-
Mouse scroll wheel + shift pan left to right
-
Auto pan is also good and happens while performing and action for example placing a component (holding shift speeds up the auto pan).
PCB/Schematic inspector
These are great tools for editing multiple parameters of multiple items at the same time. To make them appear on your side bar go to the bottom right of your window and click either PCB or SCH then click either PCB / SCH Inspector. Alternately you can go to View —> Workspace panels then SCH/PCB inspector. Then all you need to do is select a few things and edit away.
Help everything is greyed out.
If everything in your design space has turned grey you have probably applied a filter hit the clear button in the bottom right and all should return to normal.
