Schematic designator location for custom components

[Christe4nM]

My project required me to create some custom components. One thing I cannot figure out is how to define the location of the custom component designator in the schematic. When using a component from Altium’s library the designator is usually placed in the top-left corner. That’s where I want it for my components as well. Yet it doesn’t do that. I tried copying an existing component and work from there; doesn’t work either. Trying Google for about a day now has been no help at all, so hopefully someone here can help me.

See the examples below for what I mean.

Thanks in advance,

Christean

[Psi]

I wonder if its related to component center and position 0,0 in the design area?

EDIT: Na, i just checked that, doesn't seem to matter.
All the components I've created get the designator in the normal top-left position and i did nothing special to make it happen

I have no idea why you're having that issue, sorry.

[David_AVD]

I may be missing the point, but does it really matter?  I always end up shifting the designator and comment to where I want them anyway.

[AlfBaz]

in the libraries schematic editor right click an empty spot and select options->default primitives. In the primitive list dropdown box, select library objects. Have a play around, or reset you comment and designator values. Curiously mine both say
Orientation - 0 degrees
Autoposition is checked
justification Bottom left

[Christe4nM]

I may be missing the point, but does it really matter?  I always end up shifting the designator and comment to where I want them anyway.

Well, to each their own, but I don't like to do that. I like the designator and parameters placed as specified in the library. There's enough moving around already and I don't like to move them for each and every part over and over again at each placement. YMMV.

in the libraries schematic editor right click an empty spot and select options->default primitives. In the primitive list dropdown box, select library objects. Have a play around, or reset you comment and designator values. Curiously mine both say
Orientation - 0 degrees
Autoposition is checked
justification Bottom left

Thanks, for your reply. I'v been trying several settings for both Mil and MM; either overriding the library settings or not; checking the "permanent" tickbox or not; resetting; trying again. Unfortunately up to now neither seem to have any effect  I'm not ready to give up though, there must be something that sets it right, right?

[Christe4nM]

After experimenting a lot I found out that some of my components did have the designator at the top-left corner. Delving deeper they had one thing in common: the default comment was set on. So I tried that for the other components and "whadda-ya-know": that did the trick.    (Except for the Video DAC which has pins at the top side as well. But that's only one component instead of many.)

Concluding: make sure there no pins located at the top side, and set the default comment on

[marshallh]

BTW the ADV7125 is available in the vault already, save you some time..

[David_AVD]

I may be missing the point, but does it really matter?  I always end up shifting the designator and comment to where I want them anyway.

Well, to each their own, but I don't like to do that. I like the designator and parameters placed as specified in the library. There's enough moving around already and I don't like to move them for each and every part over and over again at each placement. YMMV.

Maybe I'm just used to shuffling things around for maximum readability.  A few seconds shifting labels is worth it to me.   

[Rufus]

Well, to each their own, but I don't like to do that. I like the designator and parameters placed as specified in the library.

Which guarantees they will be in the wrong place and/or have the wrong orientation or alignment when you rotate the component or flip it in X or Y.

[cpirius]

Just wanted to post the solution that worked for me since this thread is high in the google search results.

When in the schematic lib editor, right click on empty space and go to Options->Document options. Check "Always show Comment/Designator". The designator should now show up, double click it and uncheck "Autoposition". Now the designator should show with a dot next to it. Position it manually where you want it on the schematic part and it should show up in that place (and rotate correctly) when you use the part in a schematic.

[emlclcy]

I'm having the same problem with defining where comments and ref designators appear. I know this is an old link but still relevant.
One image shows the component in the library, the other image shows the result in the schematic after doing a tools>update from libraries.
In the library part I have autoposition switched off but something still overrides this once reloaded into the schematic
any ideas folks?
cheers
carl

[thekeystoneclimber]

I know this is old, but I had that same problem and and could not find the solution across multiple forums.  The key is to first set the exact position you desire for the parameters (designator, comment, etc.) in the symbol and save it.  The positioning for these is controlled in at least 3 different locations.  The first is the symbol level properties. (right click parameter -> Properties -> Autoposition)  I'm not entirely sure this setting actually does anything as it seems to be overridden by the system preferences. (this might be an artifact that Altium forgot to remove)  The next location that this is controlled by seems to be the most important. (System Preferences -> Schematic -> Defaults -> Primitive List...)  In the Primitive List, deselect the Autoposition setting for both Comment and Designator.  This will now allow components to be placed in a schematic with their parameters placed exactly as saved in the symbol library.  The final location that controls this is more related to Engineering Change Orders. (right click component -> Part Actions -> Update Selected From Libraries -> Settings -> Actions -> deselect Preserve Parameter Locations)  This allows manually positioned parameters in the schematic to be forced into the parameter position saved in the symbol library.  The caveat to being able to precisely position the parameters as intended by the symbol design is that they will not be auto-positioned upon component rotation.  Hope this helps someone.