• Welcome to our site! Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

Altium problems...Schem and library

Status
Not open for further replies.

Flyback

Well-Known Member
HellI am doing a schematic in Altium, and am having the following problems…any ideas, or a good demo video much appreciated?........

When I have drawn a net, which has a 90 degree bend in it, sometimes I wish to delete just one “straight” of the net, but in Altium I find I hit delete and it deletes the entire net when I only wanted to delete one “straight” of the net. This is easy to do in Eagle, but not in Altium.

Sometimes I want to move an entire section of the circuit to the right or left…..so I select it, then go EDIT->MOVE->SELECTION, and then I move it, but it always breaks off several of the nets, and so when I have moved the subcircuit, I then have to go round repairing all these broken nets…..This doesn’t happen in Eagle, Eagle always “knows” that you want to move a subcircuit and still keep all the nets intact.

When I want to move a component in a schematic I find that I have to repeatedly click and re-click a component before I have successfully “grabbed” it. Is there a way to “grab” it first time? In Eagle, you simply have the “axis” layer on (I can’t remember if “axis” is actually the correct name for it), and then you can see the little cross-hairs on the component, which are the places where one should “grab” the component when wanting to move it….How do you know where to ‘grab’ a component in an Altium schematic.

When drawing a schematic, I sometimes want to adjust say a 28 pin IC……perhaps I want to make all the pin names to a size 6 font instead of a size 10 font…….to do this I have to go through every pin one by one, and adjust all of the names. Is there a kind of “macro” facility where I can program it so that when I click the pin it automatically converts the pin name to a 6 font?

Sometimes I have drawn a schematic and then I want to adjust say an IC’s library symbol, and have the adjusted one on the schematic instead. At the moment I have to delete the library symbol from the schematic, then adjust the symbol in the library, then bring the newly adjusted symbol back into the schematic and reconnect it in. In Eagle you can just “update” a symbol from the library, and it updates it without you having to delete it…….how to do this in Altium?

In Eagle, you have a file which has all your favourite settings in, and you just load it (its like a workspace), and then all those settings apply……eg the schematic editor grid set to 0.1 inch etc etc….where is this file in Altium?

In Eagle you can put text on to a schematic , and that text can be multi-line text…how do you do this in Altium? In Altium I only seem to be able to get a single line of text.
 

spec

Well-Known Member
Most Helpful Member
In Eagle, you have a file which has all your favourite settings in, and you just load it (its like a workspace), and then all those settings apply……eg the schematic editor grid set to 0.1 inch etc etc….where is this file in Altium?
Hy Flyback,

I don't know the answer to your question about Altium, but I am pretty sure you can do what you want.

When you have time, can you describe how you set up the Eagle configuration file that you mentioned above.

spec
 

Flyback

Well-Known Member
Thanks, yes ill get it for you soon. Mind you, ill have to think back, because eagle is so easy and straightforward to use, that you rarely have to fiddle with such files. The schematic i am doing now, if i was in eagle, i would have finished it ages ago.....Altium is great but there are few good tutorial vids for it.

Also, how do you break and re-shape wires in Altium, -as I have layed down wires in the schem and now want to re-route them as they are now in the way…this is very easy and obvious how to do in Eagle.

Also, I am doing a schem in Altium, and making the library schem symbols, and I have just realised that I have forgotten to put in a placeholder for “package” in the component dialog box of an MMA0204 resistor…in Eagle its simple, you just go back into the symbol library, pull up the component, and put in a text for “package”, ..then go back to the schem, click the component and click “update from library”, and it updates……this doesn’t work in Altium….its very obtuse. Any ideas how to do this.?

I cannot even download a free (limited) version of altium to practice on at home, as there is no free version...and my free trial timed out months ago.
 
Last edited:

DerStrom8

Super Moderator
Most Helpful Member
Hi Flyback,

HellI am doing a schematic in Altium, and am having the following problems…any ideas, or a good demo video much appreciated?........

When I have drawn a net, which has a 90 degree bend in it, sometimes I wish to delete just one “straight” of the net, but in Altium I find I hit delete and it deletes the entire net when I only wanted to delete one “straight” of the net. This is easy to do in Eagle, but not in Altium.
First of all, stop saying "net" when you're only referring to a few sections of tracks. Nets refer to the entire electrical connection. You can have hundreds of tracks on a single net. Anyway, how are you trying to delete the track? All you need to do is click it once to highlight it and then hit "delete". Sometimes, if Altium doesn't know what you're trying to select, it will show a popup window allowing you to choose which item you're trying to select. For example, if you have a track running under a component, and you're trying to select the track, how does Altium know if you're trying to select that trace or the component that's on top of it? So, it pops up with a window showing the items it thinks you might be trying to select and you can choose the right one from there.

Sometimes I want to move an entire section of the circuit to the right or left…..so I select it, then go EDIT->MOVE->SELECTION, and then I move it, but it always breaks off several of the nets, and so when I have moved the subcircuit, I then have to go round repairing all these broken nets…..This doesn’t happen in Eagle, Eagle always “knows” that you want to move a subcircuit and still keep all the nets intact.
I'm not entirely sure what to tell you here because I don't know which "nets" (TRACKS!) are "broken off". Screenshots would be very helpful. It sounds to me like you're not selecting ALL of the tracks in the sub-circuit. Sometimes some tracks are hidden under or next to tracks that are selected, and it's difficult to tell that they're not selected.

When I want to move a component in a schematic I find that I have to repeatedly click and re-click a component before I have successfully “grabbed” it. Is there a way to “grab” it first time? In Eagle, you simply have the “axis” layer on (I can’t remember if “axis” is actually the correct name for it), and then you can see the little cross-hairs on the component, which are the places where one should “grab” the component when wanting to move it….How do you know where to ‘grab’ a component in an Altium schematic.
You can click anywhere on a component body in an Altium schematic to select it. I don't know what you're doing for it not to recognize your click. What component(s) are you having trouble with? Are you sure your mouse button isn't just wearing out? Any time I click anywhere on the component it selects it immediately. It doesn't require that you select the exact center like Eagle does.

When drawing a schematic, I sometimes want to adjust say a 28 pin IC……perhaps I want to make all the pin names to a size 6 font instead of a size 10 font…….to do this I have to go through every pin one by one, and adjust all of the names. Is there a kind of “macro” facility where I can program it so that when I click the pin it automatically converts the pin name to a 6 font?
This is easy enough. Double-click on the component to open its properties, and in the "Graphical" section uncheck the "Lock Pins" box (if it's not already unchecked). Then close the dialog, right-click on one of the pins on the schematic component, and select "Find Similar Components". The window that pops up shows all of the attributes of that one pin and allows you to select other parts with any of the attributes you choose. In your case, make sure "Object Kind" is still set to "Pin" and that the dropdown on the far right is set to "Same" (it should do this automatically) and then under the "Object Specific" heading set the "Owner" to "Same" (it defaults to any). This says that you will select ALL pins that are owned by that particular component. Make sure the "Select Matching" checkbox at the bottom is checked, and click OK. The SCH Inspector should pop up, and all you need to do is change the "Pin Designator Font Mode" from "Default" to "Custom". This will open up a couple of other settings that you can change ("Pin Designator Font" is the one you want) and the changes you make will be applied to all of the pins in that component.

This sounds complicated, but once you do it a couple of times it will become second nature to you. When you understand how the SCH Inspector works, it'll be very obvious.

Sometimes I have drawn a schematic and then I want to adjust say an IC’s library symbol, and have the adjusted one on the schematic instead. At the moment I have to delete the library symbol from the schematic, then adjust the symbol in the library, then bring the newly adjusted symbol back into the schematic and reconnect it in. In Eagle you can just “update” a symbol from the library, and it updates it without you having to delete it…….how to do this in Altium?
You do not have to delete the part from the schematic. Update the library component, then when you have the schematic editor open simply go to Tools --> Update From Libraries. Select the component you want to update from the list (check the box next to it) and click Next, then Finish. It will pull in the changes from the library into the schematic. No need to touch the schematic component.

In Eagle, you have a file which has all your favourite settings in, and you just load it (its like a workspace), and then all those settings apply……eg the schematic editor grid set to 0.1 inch etc etc….where is this file in Altium?
Go to the DXP menu --> Preferences, make sure all of your favorite settings are selected (for example, grid size in the Schematic section), then at the bottom click the button that says "Save...". This will prompt you to save your preferences file (xxxxxxxx.DXPPrf). You can then load the settings from this file later by going to the DXP menu --> Preferences --> Load...

In Eagle you can put text on to a schematic , and that text can be multi-line text…how do you do this in Altium? In Altium I only seem to be able to get a single line of text.
In order to create multiline text on schematics you'll have to use a text frame. I don't like it much, personally, but it does the trick. Go to the Place menu --> Text Frame (shortcut P-F). Personally, I hope they add multiline text functionality in the main Place --> Text command (P-T) like they did in the PCB editor. I usually just end up placing individual lines of text because I don't care for the text frame.
 
Last edited:

Flyback

Well-Known Member
Regarding adjusting the routing of nets in the Altium schem editor, the “break wire” command does literally that…..which is unfortunate, in Eagle, “break” puts a kink in the wire which the user can easily grab hold of and quickly and simply “mold” the wire into the required routing position. Surely such a facility must be available in Altium?

By the way DerStrom8, your excellent video on Altium was the only reason i got off the ground in Altium at all....i used to watch it on my amazon fire.
 

DerStrom8

Super Moderator
Most Helpful Member
Also, how do you break and re-shape wires in Altium, -as I have layed down wires in the schem and now want to re-route them as they are now in the way…this is very easy and obvious how to do in Eagle.
This does appear to be a shortcoming, unless there's a tool I'm not aware of (which isn't entirely unheard of). To my knowledge, the only way I know of to do this is to manually add a vertex to the wire, which is kind of a PITA. Double-click the wire and select the "Vertices" tab, click "Add..." and set the X/Y values. You can then drag using this vertex. It's a bit of a pain to do if you plan to drag a lot of wires around. Personally I prefer to use net labels instead of long wires. It's much cleaner and much more professional.

Also, I am doing a schem in Altium, and making the library schem symbols, and I have just realised that I have forgotten to put in a placeholder for “package” in the component dialog box of an MMA0204 resistor…in Eagle its simple, you just go back into the symbol library, pull up the component, and put in a text for “package”, ..then go back to the schem, click the component and click “update from library”, and it updates……this doesn’t work in Altium….its very obtuse. Any ideas how to do this.?
You can update from libraries the same way I mentioned in my first response.
 

DerStrom8

Super Moderator
Most Helpful Member
By the way DerStrom8, your excellent video on Altium was the only reason i got off the ground in Altium at all....i used to watch it on my amazon fire.
I appreciate that Flyback. As I think I mentioned I plan to make more, but I just haven't had the time.
 
Status
Not open for further replies.

Latest threads

EE World Online Articles

Loading
Top