Draftsman in altium

Hi everyone,

I didn’t have lot of time these past few days but I am back to show you some good things using the tool Drafstman in Altium.

Have you ever wanted to produce a nice document related to your design but you don’t know where to start? I mean, a document which look like professional where you can put all your engineering requirements and mechanical informations.

Draftsman is what you need.

Draftsman is an alternative way to create documents for board design. Based on a dedicated file format and set of drawing tools, the Draftsman drawing system provides an interactive approach to bringing together fabrication and assembly drawings with custom templates, annotations, dimensions, callouts, and notes.

Once your design is finished, you can add a Drafstman document by clicking on New->Drafstman document:

As you don’t have any template yet, you will have to choose an empty sheet (Default) for your first one:

You can start by changing the page option, sheet size, grid…

Then the fun can start!
With the Version 18, Altium make some improvements. You can have more choice in the place section.

I like to place an isometric view which is nice for an overview of the board on the front page:

Then you can place a frame with information like title, number of page, date, author…

A cool trick that you can clic on the (x)+ button to acces to the list of parameters used in your design:

For example to get the number page you will write:

Page =SheetNumber / =SheetTotal

After that you can add more sheet by clicking right and « add sheet ». You can add more views of your PCB, the stackup, the drill table, your BOM and more…

If you like your arrangement you can save it as Template by clicking on File->SaveAs and choose:

Once you finish, you will be able to export the Draftsman document in PDF clicking File->Export->PDF

Here we go, I hope this will be helpful 🙂

How to generate a STEP 3D File without small components (reducing the size of the file)

During a product design, you are sometimes brought to work with other designers. To do a well assembly with mechanical part like casing, harness cable… you will probably have to share your design using STEP 3D files. A big problem when you are doing a complicated design is that the 3D STEP can quick become a heavy file (>100mo).  This can be difficult and annoying to send or share (via mail/FTP server) especially when you send your design back and forth to make small corrections…

To reduce the size of the file, the best way is to remove all 3D parts that you don’t need. Generally we use 3D step to make sure everything is well centred, aligned and the design fit correctly and the connectors match with the rest of the design. This means we don’t need to add the 3d models of small packages like 0402 resistors for example. Don’t forget that more 3d models you have, bigger the size of the file will be!

How to choose only big packages?

    • First open your PCB, in 3D or 2D view whatever (in my example I am using the OpenRex Project from imx6rex).
    • Then click on the Panel button on the right bottom side and open the PCB Filter

  • In the filter write : IsComponent and (Height >= 50) 

You can adjust the Height value depending of your needs and if your design is in millimeter or in inch.Don’t forget to check the box Matching: « Select ».

 

  • Now click on « Apply to All ». At this step, all the components that are bigger than your threshold are selected.All you need to do to finish is to click on File->Export->STEP 3D:

  • In the opening window (Export Options) you have to choose « export selected ». This will create a step 3D with only selected components.

  • Here we are, we have now a 3D STEP file definitely lighter than the original one!:

Problems

Components are not selected with the filter!

You will probably be face to this problem, you should know that this problem is not a bug from Altium, but it’s from your design! You have to understand how PCB filter works. When you use the PCB filter, the software will filter the parameter « Height ». This parameter should be filled in every PCB component that you are using.

For example, I have a USB connector, as you can see the Height of the connector is 118mil, it’s correct. The PCB Filter will select the connector when using « Height >= 50 ».

Another example with a SD card slot, you can see that the parameter Height is 0, this means when you will use the filter, as the height is zero the component wont be selected!!:

In conclusion, make sure that all you component have a Parameter Height with the right value before using the filter.

Leave me a comment if you have any questions or if it was helpful. 😉

How to add a quick table of contents in Altium

There are several ways to add a table of contents in your Altium’s design. The more personalized will be probably to do it by hand but it will take you a lot of time to adjust everything in order.
In this tutorial, I am going to show you an easy way to make a quick table content in Altium using directly a copy of the Annotation compiled sheets window.

In this example I will use the OpenRex Project from imx6rex.

  1. The first step is to numbering all your sheets if you did not do it.
    Go to Tools->Annotation -> Number Schematic Sheets
     In the opening window, click on the « Update Sheet Count » button to update the number of pages, then put your sheets in order and press « Auto Sheet Number » and « Auto Document Number ».
  2. Now that all your sheets are numbered, go to Tools-> Annotation-> Annotate Compiled Sheets.
  3. Put in order all of your sheets using the MoveUp and MoveDown buttons then click on « Annotate Sheet » to update the sheet number row.
  4. Guess what, this table will be your table of content! Select all the table using Shift+Click the Ctrl+C to copy the table.
  5. Open a new spreadsheet (Open Office, Excel…) then paste the table:
  6. You can add all you want, images, colours… Once you are done, just copy and paste the new table to your first sheet design using Ctrl+C, Ctrl+v
  7. Here is an example of final result (I am sure you can do better):
  8. Leave me a comment if this was helpful. 😉

Altium designer 18

Here we go, the new version of Altium 18 is out since December 2017.

You are still hesitating to make the step and  go to the 18th version ? 

Read my article to know everything you need before switching to the new version.

The new interface

The company decided to completely remodel the new version with a new interface  which looks modern and fresh with the grey/black background. All (or almost ) functions that were in earlier versions are there, however they made the decision to move the position of  some tools from left to right. Why did you do that guys?!

For example, the system preferences and the profile/licence management were always on the top left of the windows, now it’s on the right.


The first times you will use the software it create confusion or annoyance. You will not be able to find what you are looking for just as in earlier versions.  The hardest part is to forget about your habits that you used for decades from Protel to Altium designer 17.

A good new feature is that all the properties are now displayed as a non-modal window, this means that you are no longer forced to right click on a component to change his property (this will save you a lot of time when you want to move coordinate ‘s component, write text, change layers…). The non-modal window from the tab panel show directly all the information of the component:

Other than the new interface they finally allowed designers to do assembly multi-board.  The first step is to create a workspace that contains several projects. After that you will have to create a new schematic containing the pin out of the connection between boards.

This is definitely an improvement, who never made mistakes and got two boards that could not fit together or with a wrong pin out connector?! With this new feature you will be able to generate a report and make sure you two boards are synchronous. With the 3D assembly you will be able to see any design mistakes like the height of a component that touch the other board, two screw holes that are not well aligned and more…

In terms of performance, Altium did a big advance compared to version 17. The transition from 2D to 3D is  so smooth particularly thanks to the multi-threaded tasks and the fresh 64 bit architecture. The software will take all  the resources needed to run smoothly and fluently.

Active route

Altium wants to save your time while designing your board with this new feature called Active Route where the software handles the design constraints, such as the clearances, widths, vias …  This will reduce one of the most time consuming phases of your layout. You are going to wonder what is the difference with the autoroute? Well this feature is definitely more efficient as it just apply for your specific nets or component and not to all the board as an auto router would do. More over you can very easily define a path where the traces will flow.

PDN Analyzer

Power delivery network (PDN) Analyzer is an extension not powered by Altium but by CST® . This extension was available for Altium 17 but it looks like they really want to promote PDN Analyzer with the new version of Altium 18. PDN is a simulation tool, which analyzes a board design’s DC performance based on its electrical and physical properties. I wouldn’t go any further about PDN Analyzer on this article. I thing this tool needs his own post, stay tuned!

 

In conclusion, the update to version 18 will depends of your needs. If like me you were frustrated not to be able to assembly two board together you should go for Altium 18. All the new improvements make the design easier and time-saving, however it will take a little period of adaptation to fully take advantage of the new interface. And finally, as always when new released are out, lots of bugs are found and corrected  so make sure to check frequently for new corrected/fix update.

Al.