Altium PCB Design Preference questions

[RaylonS]

Hey gang, I'm working on my first few layouts in Altium, having completed one. I was hoping I could get a few tips on what (in my experience with OrCAD) were relatively easy things to do. Please chime in with whatever bits you have knowledge of.

1) Is there a way to force the display to show 'hollow pads'?
Instead of filling a pad with solid copper which obscures trace endpoints, is there a way in the display only, to show the pads as outlines?

2) Is there a way to lock into 'routing mode'?
I am finding it very tedious to have to choose between a trace I want to modify and whatever other obstacles might be in the vicinity when I am trying to route a board. I get the little pop-up that lets me choose the track I want, but if I'm routing, why would I want to select a component, a pad, or an obstacle? I find this wastes a lot of time and would like to know if there is a dedicated 'routing mode' so I don't have to type P,T every time I want to grab lay down a new trace.

3) How can I SELECT an entire trace (not just track/segment)?
CTRL+Click highlights, but does not allow me to edit the trace properties through the PCB Inspector. And I know I can shift+click to grab each track individually, but this can be very tedious if, for example, I just want to delete, or change the width of a long, multi-segment trace.

4) How can I ensure components are NOT inadvertently modified during placement/routing?
I have not found in Altium the equivalent of OrCADs 'Allow Editing of Footprints' which can be set to On or OFF. Is there a way in Altium to ensure I dont accidentally grab an object that's part of a footprint and move or modify it, thus messing up the footprint? In other words, 99.9% of the time I have no use for editing footprints once I'm in the layout, I should be able to turn 'edit footprints' off.

Being only a few months into my experience, these are some basic things that would save me a lot of headache and help ensure I'm not introducing errors into my design.

Thank you for any input
Raylon

 

[kevin54]

Here's a link to some helpful tips:

**broken link removed**

For questions 3 & 4, you click on an object (say, a component or trace), then right-click -> Find Similar Objects. If you want to select all components, set "Object Kind" to "Same", click OK and it will select all components and bring up the PCB Inspector. Click the "Locked" box and it will lock all components. Similar idea on changing track widths, select a track, Find Similar Objects after setting "Net" to "Same", then change the track width in the PCB Inspector and all selected tracks will change. If you want to enforce a track width (i.e. power or ground) you should create a "Width" design rule for those nets.

 

[RaylonS]

Thank you for your feedback.

I did read through Johns Blog tips, but it doesn't really say anything that directly addressed my issues such as hollow pads or a dedicated routing mode.

I am familiar with the find similar objects, but I was hoping there was a more streamlined way to simply select a trace than to click one segment, right click, choose find similar, set net to Same, set layer to same, click OK. (thats like 9 clicks!)

Plus if I had other traces on that net on that layer, how could I may need to exclude them from my selection?

So for 4 you feel that the only way to prevent footprints in a design from being editable is to lock them? This is better than an accident, but then if I need to slide a resistor this way or that while routing I have to unlock it first.

This may be related, can you define for me 'primitive object'? Is a line of a silkscreen or a pad of a component 'primitive'? Or is the component itself 'primitive'?

 

[kevin54]

For (1), You can use "View Configuration" to set Pads to display in Draft mode: Control-D -> Show/Hide Tab -> Pads = Draft; You can create a new view configuration, name it ("Draft Pads"?, and it will be accessible from the pick list on the toolbar.

(2) If you are in "Interactive Routing Mode" (click the tool, or Place -> it won't offer to select obstacles, etc., it will only let you route. If you're not in Interactive Routing Mode, if you click in an ambiguous place, it insists that you tell it which object to select. I don't know of any way to prevent this. I try to click in unambiguous places if I can.

(3) You can change track widths in somewhat fewer clicks by Selecting the Net (keyboard shortcut "SN", then click on the Net). This will select everything on the net. You can filter for Tracks (define a filter shortcut for "IsSelected and IsTrack") then change the Track width in the PCB Inspector. I don't know of a shorter way, but in any event it's best to plan your track widths before you route, and set rules for them so they route with the correct widths and are enforced by Design Rule Check.

(4) If "Lock Primitives" is set for all components (it should be by default, if not you can set it in the inspector)) you shouldn't be able to accidentally edit parts of a component, only move the entire component.

 

[RaylonS]

Thank you for your additional feedback. I will check out these settings and alternate commands and experiment with locking the primitives/components