Actions
Forum Thread Details
  • State Suggested Answer
  • Locked Locked
  • Replies 10 replies
  • Answers 1 answer
  • Subscribers 91 subscribers
  • Views 1419 views
  • Users 0 members are here
Related
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

Creating a board outline - where are the CAD tools

cpallan

I don't see a way to create a complex board outline in Circuit Studio. There are only freehand tools, no CAD type tools for outline / mounting holes. Are there tools - am I missing something?

 

Thanks,

Charlie

  • 0

    I generally use the method of creating the board from defined objects.  I create the outline using a Keepout or something else that is easy to draw, measure and adjust.  When I've got the right shape, I select the outline in single-layer mode and define the board from the selected objects.  There might be times when I need to adjust the board shape in the middle of a project so it's really handy to keep the board outline as its own layer so I can set it to single layer mode and easily highlight the outline and redefine the board shape.

  • 0

    Or use a real mechanical CAD tool to do the shape, bring either the enclosure or board model in as a step file and take the board shape directly off that (there's a tutorial by Altium for that).

  • 0

    agreed - there isn't a good cad tool in CS for doing outlines.  I do my outlines in solidworks...  (bringing a nuke to a knife fight?)

  • 0

    maybe you can use the 'free' autodesk cad tools.  i'm not familiar with those, but i expect you could get a board outline made.  I did my board outline using solidworks, exported a step file, imported that step as a library component in CS, placed that part on my PCB, then press '3' to activate 3D view mode, then you can 'create board outline from 3D shape'.  ultimately I got what i wanted, but like I say - solidworks is like at minimum a $4k software, and CS a pcb CAD tool ought to have some better polygon definition tools beyond the not so grid snappy, 45 degree imposing more or less free form box drawing tool.  it'd be good for a lot more than just PCB outlines.  a dimensioning tool similar to solidworks sketches would be just brilliant.

     

    as a side question, does altium designer have a better CAD sketching tool?

  • 0 in reply to mflux_gamble

    Unless something has change in the latest AD release, what's in CS is the same as AD for mechanical CAD sketching (if you can even call it that.)

     

    I use Fusion360 as I qualify for their free licence as a startup. I find it does everything I need for enclosure design through to CAM, but I really only do 2.5D stuff.

  • 0

    Besides complex shapes...  there does not seem to be any tools for simply adding mounting holes.

    I would have thought this is required in almost every design.
    Please tell me if I have missed it.

  • 0 in reply to awardautomation

    For mounting holes, I just place a through-hole pad with the pad size set to the same as the hole size and no designator. I believe that is the most common approach but could be wrong.

  • 0 in reply to adamwebber

    This method works for me, also. It is also fairly easy to 'snap-in' board outlines with the regular layout tools, although not as easy as in a CAD app. First, set your Origin at some convenient datum point, so that X,Y values can be taken directly from a drawing. Set your snap grid to values convenient for the task. For example, if you have a lot of outline features at coordinates like 10.5 mm, set Snap Grid to 0.5 mm. You might want to change the Snap Grid settings more than once during the process. If you have rounded corners, set the routing mode for generating rounded corners and adjust the Design Rules for a suitable radius. Once you have the outline on some layer, you can select all objects and use the 'Outline from Selected Objects' command. Interior cutouts seem to require a separate operation, but can be done similarly. Use 'Place Pad' to create holes at particular locations. Set Pad Size and Hole Size to the desired diameter, and set the Plated Through option as required for the hole. Use 3D View to easily see what you have modeled and to look for missing features or errors. When the holes are setup properly, for example, you will clearly 'see through' each hole to the background color. You can use the 'View Configurations/View Configuration' command to adjust layer colors. I choose realistic colors, so that the 3D view does a decent job of rendering the assembly.

  • 0 in reply to awardautomation

    You can design a mounting hole as a component that is just a through hole pad.  Then add clearances and keepouts as needed (for screw heads, washers, tool access, etc).  You can build up a library of these for #4, #6, M3, M2.5, etc fasteners or for plated and non-plated mounting holes.  IPC-7351 has a naming convention for mounting holes that makes it somewhat easy to assign and then figure out what these are.

     

    Once you have a schematic library and footprint library you can put the mounting holes on the schematic and then treat them like any component in the process.  This lets you have an electrical connection to a mounting hole if you want to use it for chassis ground.

  • 0 in reply to mflux_gamble

    Hi Mflux

    Are you able to provide more detail on how you import a step model?

    Ive modeled the enclosure and board in Fusion360, then exported the board as a step model,

    but just cant figure out how to import it into CS.

     

    Its probably really simple, Im just overlooking something