| T O P I C R E V I E W |
| rvpilot |
Posted - 15 Apr 2016 : 17:58:33
I've added a copper shape to a pad and associated it using "Link to Pad Number" ... now, I know this suppresses the DRC and gives the shape the same net allocation as the pad, but when I produce my Resist and Paste layers, only the pad itself is used to create the mask ! So, useful for heat sink copper, etc, but not useful for creating odd shaped pads, i.e. under power inductors, etc.
Does any one know how to get the behaviour I need ... I suspect its through an exception? or is it not possible at all :-(
Would be a nice feature (for v20 ... hint hint) to add another check box to the shape properties such as "Resist/Paste Layer - Treat as Pad" or something more friendly! |
| 6 L A T E S T R E P L I E S (Newest First) |
| John Baraclough |
Posted - 16 Apr 2016 : 19:20:49
Glad you got it working.
-------------------------------------------------------
Birthdays are good for you: the more you have, the longer you live ... and I've had lots of them so I should know! |
| rvpilot |
Posted - 16 Apr 2016 : 13:09:00
Thanks for the pointer John, I had defined the same Layers in both PCB Symbol and PCB Editor, but the Layer Types associated with those layers did not share the same name between Symbol and Editor. Its the Layer Type name that is used, not the layer name itself !
Many Thanks :-) |
| John Baraclough |
Posted - 16 Apr 2016 : 12:52:24
It sounds as though you haven't added the new layers to the design technology file for the board.
Go to: Settings -> Design Technology.
Click the "Layers" tab.
Click the "Add" button and create the appropriate layers.
-------------------------------------------------------
Birthdays are good for you: the more you have, the longer you live ... and I've had lots of them so I should know! |
| rvpilot |
Posted - 16 Apr 2016 : 11:00:39
I've gone into the PCB symbol and added a shape (slightly bigger than the pad).
I've added 2 new layers in the PCB symbol called "Top Paste" (type="Paste Mask") and "Top Resist" (Type="Solder Mask").
Now I assign the shape to Layer="Top Resist" and the shape colour changes as per the layer definition.
Added a shape smaller than the pad and assigned to Layer="Top Paste".
All Good so far !!
Now, going back to my design, then update component and the new shapes don't appear on the PCB editor, nor do the get picked up when creating output plots ! Any clues as to what I'm doing wrong or is this not the right approach ?
EDIT : I notice that in the Add Component preview, the PCB symbol shows the resist and paste shapes, deleting the old componet and re-adding to the design still doesn't show the shapes in the PCB editor. It does show the resist for all my other components though!?
EDIT : I have a component created in 2012 using this same technique and that works as expected ! So something has changed/broken in an update since then !
I have also noted that the "Shape Draw Order" does not work .. it just seems to draw them in the order they were first added :-( EDIT : Ignore that, this only works for item on the same LAYER ... otherwise the layup order defined in the Layers table kick in !!! DOH! |
| John Baraclough |
Posted - 15 Apr 2016 : 20:17:46
You can get more flexibility with mask and paste layers if you create them as separate layers in the design technology file rather than using the default oversized and undersized pads. If a separate layer exists, plotting and printing will use it instead of the default.
You can put text and symbols into the mask layer if you wish which is how I did these panels:
http://mydesk.myzen.co.uk/_Useful/BlueCom/BluecomBeltpackFront.jpg
http://mydesk.myzen.co.uk/_Useful/BlueCom/BluecomBeltpackBack.jpg
-------------------------------------------------------
Birthdays are good for you: the more you have, the longer you live ... and I've had lots of them so I should know! |
| Iain Wilkie |
Posted - 15 Apr 2016 : 18:56:08
Yup, you simply create the shape you want on the resist and paste layers when you create the component.
Iain |
