Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

Altium Designer 6.6 basics

Status
Not open for further replies.
N

nzkunal

Member level 2
Member level 2
Joined
Mar 11, 2004
Messages
52
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,286
Activity points
377
altium jump component shortcut

Hi,

Does anyone know if there are short cuts to search for parts / components in schematic and PCB view for Altium 6.

Havent been able to find anything in their shortcut guide...

Thanks,

Kunal
 

When you are working in the schematic or PCB editors, you can use "JC" (jump component). A dialog will come up allowing you to specify the designator to which you want to jump.

Another way is to use the PCB Panel in the PCB Editor. Set the panel to "Components" at the top, click on "All Components", and then select the one you want from the list in the middle panel. When you click on the component name in the middle panel, the view will zoom to the part on the PCB. The Navigator Panel in the Schematic Editor works in a similar way for the schematic.

You can also turn on the "Cross Select Mode" found in the Tools menu. If you turn on that mode in both the schematic and PCB editors, whatever you select in one editor will be selected in the other.
 

    N

    nzkunal

    Points: 2
    Helpful Answer Positive Rating
thanks for that was aware of the second one but the JC shortcut was exactly what I was after!

Another question: How do you set-up via sizes and quickly toggle between alternate via sizes when routing...
 

I can't recall which version of AD introduced the favorite via table. If it's available in version 6.6, you can hit Shift+V while placing a track interactively (PT). A table of vias will come up from which you can select your size. That table is edited from Preferences>>PCB Editor>>Interactive Routing.

There's also a table for track widths that can be brought up with Shift+W.

All of those shortcuts can be found by hitting "~" while using a function. For example, hit PT, start placing a track, and hit "~". A table of shortcuts will come up.
 

    N

    nzkunal

    Points: 2
    Helpful Answer Positive Rating
Is there anyway to turn off the visibility of comments for multiple objects. There doesn't seem to be an option in the sch inspector...
 

You hide a group of comments like you do any other parameter from the Schematic Inspector Panel.

Select each of the comments by clicking (or Shift+Clicking). You can also use Find Similar Objects. Open the Inspector Panel - at the bottom of the panel is a section that says "Object Specific", and under it you should see "Parameter Name - Comment". In the top section of the panel is a checkbox that says "Hide". Click on that box and all selected comments will be hidden.

You can also get to the same dialog by selecting the components for which you want to hide the comments, then going to the Inspector Panel. Click where it says "Part Comment" in the left column. A new dialog will expand for just the comment strings. You then check the "Hide" box just like the first method I outlined.
 

    N

    nzkunal

    Points: 2
    Helpful Answer Positive Rating
Hi,

How do you change the selection of track widths that come up when Ctrl+W is pressed during interactive routing?

Also am trying to change the width of multiple tracks is there any way to select nets between two pin pairs rather than selecting each individual segment?

Thanks
 

The table of preferred widths is changed/edited from Preferences>PCB Editor>Interactive Routing. There's a button at the bottom of the dialog for widths, and another for via sizes.

There are several ways to select a net, or portions of a net. "SC" (select physical connection) will select all routed track between two pad objects. "SN" (select net) will select the entire net, and you can use "XO" (deselect outside) to deselect what you don't want. Likewise, you can use "SP" (select connected copper). You can also select a net from the PCB Panel by setting it to "Nets" and then selecting the specific net from the list.
 

    N

    nzkunal

    Points: 2
    Helpful Answer Positive Rating
Thanks for that.

I am trying to create a rectangular hole in a PCB footprint. To create a round hole I just place a Pad without an solder padding and just a round hole. I can create a square hole but how do I make it rectangular?

And is this actually the best way to create holes in a footprint as it leaves orphan pins?

Thanks,
Kunal
 

There's no such thing as a square drill bit. To create a rectangular or square hole, the fab has to route or punch the hole. If you draw the outline of the rectangular hole on the same layer as your board outline, you can specify that layer as a route path layer when you send your Gerbers to fab. Just be sure to provide a proper void around the hole on any plane layers you have. Drawn cutouts don't automatically generate plane pullbacks.

Why do you need rectangular holes instead of slots? What do you mean about orphan pins? You'll have to be more specific about your footprint for me to be of any help with that.

Speaking of help - if my responses have been helpful, I would appreciate you hitting the "helped me" button once in a while. It doesn't cost you anything.
 

    N

    nzkunal

    Points: 2
    Helpful Answer Positive Rating
Yeah decided to use slots instead.

By orphan pin I mean that for example a MOSFET schematic component has only 3 pins if I put an additional slot (for the heatsink hole perhaps) on the PCB component there will an extra pin 4 that is not used on the schematic component as it doesnt require a net. Is this normal or should the additional slot be some other type of object other than a pad?

I am trying to create a simple rectangular 3D model for a footprint I have made is there an easy way to do that? I specified the height and thought that it would create a model from the extremities but that didnt work...
 

It's OK to have an extra pad in the footprint. I usually give mine a name that matches its use - like MH1 for mounting hole, or HS1 for heatsink. Mounting holes in MOSFET devices are often internally connected to one of the active pins. You may want to consider that in your schematic representation.

It's been a while since I used version 6.6, but I think that was before the new 3D view was added to Altium Designer. If that's the case, AD will automatically create a 3D body from the component extents. You may have to rename the default 3DLib file to force the program to regenerate new bodies.
 

    N

    nzkunal

    Points: 2
    Helpful Answer Positive Rating
Is there a way to have a custom template or save settings for generating BOM's in AD6.
 

When you select Reports>>Bill of Materials, look at the bottom right corner of the dialog. You can select an Excel spreadsheet template to use for display of your BOM. Just like all the other templates used in AD, you'll find examples in the ...\Altium Designer 6\Templates folder.

BOM templates are written as Excel worksheets. You have to know how to do that, or you have to modify the exisiting templates in Excel.
 

    N

    nzkunal

    Points: 2
    Helpful Answer Positive Rating
Thanks that got me on the right track anyway I setup an *.outjob file that can be usesd accross different projects. Exactly what I needed!

Is there a way to update properties of components / parts in a BOM / tabular format for example and import that back to a schematic file.

Often I have RS components numbers / costs I want to associate with parts would be great to update these in BOM in excel and then update it in the schematic.

Thanks
 

No, you can't go backwards from the BOM to either the schematic or the PCB.

I can't remember which version of AD introduced the feature, but the newer versions have Tools>>Parameter Manager in the Schematic Editor. From that dialog, you can add and edit component parameters. It seems to me that would be the place to do what you are describing. It's a spreadsheet type of display, and you can import/paste columns of data.
 

    N

    nzkunal

    Points: 2
    Helpful Answer Positive Rating
Found it. Exactly what I wanted!
 

How do you edit sheet properties in the bottom right of most sheets.

I tried updating Document Parameters but nothing changes
 

In order for the Document Option Parameters to be displayed, you have to have the appropriate special string on your schematic sheet. The special strings are those with "=" in front of them when you look at the scroll box while using the Place>Text String command (hit "Tab" while using Place Text).

The parameters corresponding to the special strings will be displayed on your documents if you have "Convert Special Strings" checked in your Preferences>>Schematic>>Graphical Editing.
 

    N

    nzkunal

    Points: 2
    Helpful Answer Positive Rating
Hi,

Is there a short cut of enabling selection of part items only?

Thanks,
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top