It is well known that the PCB world and the mechanical world must collide and sometimes they do so violently. PCB layout tools are very well suited for layout and can do most anything necessary for drafting purposes, but they are often not streamlined for mechanical design. Therefore, knowing several ways to accomplish the same work is very helpful depending on the situation. This will be a small series that may be helpful to you when starting your next design.
Defining the Board Shape
The ability to simply draw the outline to whatever shape you would like is long gone. For this reason alone, it is reccomended that you always have a mechanical layer dedicated for a board outline. We use mechanical 1 for ease of use (M1 is how all instructions below will be referenced), but whatever you like will work. Here are various ways to define the board shapes and the most common ways to use them.
Manual Creation
If you just have a simple rectangle, it is often easiest to just draw 4 lines on M1 and then set the board shape to those lines. Here are the steps...
1. Select M1 and draw the rectangle to the desired size.
2. Use a shortcut command SY. It is for Select all on laYer. This will select all 4 lines for you.
3. Go to the menu Design->Board Shape->Define from selected objects or DSD for short.
4. Remember to clear the selection filter with Shift+C so that you can continue to work.
That's all there is to it! If you want to change the board shape, just drag a line or 2 and repeat steps 2-4 above.
Create from DXF
More complex board outlines often come to the layout specialist in the form of a DXF. For this process it is very similar to above, but now there is an import procedure for the DXF.
1. While in the PCB, go to File->Import...
2. Select the DXF file from the browse dialog
3. Select the appropriate input such as scale, line width and location.
4. If it is only the outline, you may choose to import everything direct to M1. Since DXFs often come with dimensions, showing component outlines, etc. you will probably be better off choosing an unused mech layer and then copying the board outline only to M1.
5. Once your board outline and only your board outline is on M1, the same steps 2-4 in Manual Creation can be used.
A couple of hints for this method:
1. Make a union of the board outline primitives to more easily manipulate it
2. When placing parts and mounting holes, set the active layer to where ever the DXF was imported. This way components can be picked up and snapped to the correct location.
Create from STEP model
If you get a good STEP model, it too can be used to create the board area very quickly. There is a small drawback to this method at this time though.
Mounting holes and pins of all shapes will show up and Altium saves them as free pads in a union. This is handy to snap components to, but then pieces will have to be removed as you will end up with 2 holes in one place. The same is true for mounting holes, unless they are not defined as components in the schematic. In this case though, only a plated hole comes through with no annular ring so the data will still need to be manipulated.
Still, a complex shape can be created accurately and quickly from a STEP file now.
1. Import the STEP file by going to Place->3D Body.
2. Set the top radio button to Generic STEP Model and down below select the Embed STEP Model button.
3. Browse to the file and press Open.
4. Click the location to set down the STEP model where you want it. If you miss, just move it to where you would like it.
5. In 3D mode, go to Design->Board Shape->Define from 3D body
6. A small thick cursor shows up. First click the object that you would like to use, then click the surface you would like to use. Note that while picking a surface, Altium will highlight the surface shape in blue.
7. Choose how to align the model to the board surface and click Close.
You may now exit 3D mode and clear the filter.
Create Primitives from Board Shape
To be added
Board Cutouts
Unfortunately, board cutouts don't always automatically appear when using the Define from selected objects command. If the construction lines are already down though, it should be fairly easy to trace them, snapping to corners by using the Define Board Cutout command.
1. Go to Design->Board Shape->Define Board Cutout
2. Draw the shape for the cutout tracing and snapping if possible.
3. Close the shape and check the cutout. What Altium does is define a region and set it as a board cutout. It can be manipulated/removed just as any other region.
Auto-Position Sheet
To be added
Hope this helps and happy designing,
David
No comments:
Post a Comment