0
\$\begingroup\$

The component AMS1117 comes in three packages. Then each package has a part that gives different fixed output voltage. Here is the table:

enter image description here

When creating the library for this in Altium designer, I shall have one footprint for each of the packages TO-252, SOT-223 and 8L SOIC. Then, I shall have a single schematic symbol for all the different variants for the different voltages. However, since each of these is actually a different part, this means that there will be 7*3=21 parts in schematic library that look identical but represent each of the different 21 parts. And, there will be 3 parts in the PCB library since there are three footprints. Is this correct?

This means that, it is not possible to create a single solitary alone schematic symbol called AMS1117 that when put the into the schematic, we choose the specific part (out of the 21 parts) using something in a drop down box in the properties. Is this the correct way?

\$\endgroup\$

2 Answers 2

2
\$\begingroup\$

Just create the parts you need for the design. If you're undecided on package type, you can create the schematic symbols for the three different packages.

Altium has a feature similar to Orcad's "include" feature which allows you to stuff parameters from an Excel database file in to the schematic layout. Do a search for "Database Link File" to see how to use this.

Example, I have a few schematic symbols for resistors based on footprint style such as R0402 for a 0402 resistor. I will add the value to the schematic during the design phase. Before I commit to layout I will run Tools → Update Parameters From Database which will stuff parameters like manufacturer, manufacturers part number, footprint, description, and company part number. This is matched against "Library_Reference", "Value", "Spare1", & "Spare2" which are part of the schematic symbol. Normally Spare1 & Spare2 are loaded with "." (period) to appease limitations in Altium's search engine, but sometimes I'll have special information in Spare1 and Spare2 to make similar parts unique. For resistors & capacitors, Value is left blank in the library symbol since I fill it in during the design phase. For voltage regulators, Value will contain most of the part number except the output voltage in the library symbol. The output voltage is filled in during the design phase.

The include file technique works well for solo operators and is a bit cumbersome to do in a work environment with multiple seats.

\$\endgroup\$
4
  • \$\begingroup\$ When we buy resistor, capacitor or inductor, there is a different part number for each different value resistor, capacitor and inductor. Doesn't this mean that when the resistor part is created in Altium schematic library, its value will be fixed at that time? This is because if we change the resistor value in the schematic, the actual manufacturer manufacturer part number will become different and will need to be changed, thus it will be simpler to just have a separate part for each different value resistor. Correct? \$\endgroup\$
    – quantum231
    May 15, 2023 at 13:12
  • \$\begingroup\$ @quantum231 This is why database linking works so well. For a resistor, all you need is a schematic part that matches the footprint size. The value is added during the design. When you're done with the schematic, you "update parameters from database" which will stuff the part number, description, footprint, and whatever else you desire in to the schematic parameter fields. If you change a value, rerun the database updater. \$\endgroup\$
    – qrk
    May 15, 2023 at 16:24
  • \$\begingroup\$ I have only created a basic LED based 2 layer board so far with Altium designer. I shall habe to look into what this database stuff is. \$\endgroup\$
    – quantum231
    May 15, 2023 at 16:36
  • 1
    \$\begingroup\$ @quantum231 Altium's documentation is rather difficult to follow on database linking. One thing not mentioned in any Altium documentation is the need to have Microsoft Office for database linking to work. If you don't use MS Office (i.e. you use Libre Office), you need to install Microsoft's "Access Database Engine Redistributable". Be prepared to spend a few months exploring Altium as there are many features, some not well documented. \$\endgroup\$
    – qrk
    May 15, 2023 at 17:29
1
\$\begingroup\$

The packages are probably industry-standard, so appropriate footprints will probably already be in Altium's footprint library - no need to make new footprints for this part.

I would probably just create one schematic symbol for the Adjustable version, and one for the fixed version, with each schematic symbol having your usual footprint as default, and the other two as options. For the fixed-voltage versions, I would add the voltage when I placed the schematic symbol. Or I might make separate schematic symbols for each voltage I actually use. I don't see any point in cluttering my libraries with things I won't ever use.

\$\endgroup\$
4
  • \$\begingroup\$ When we buy resistor, capacitor or inductor, there is a different part number for each different value resistor, capacitor and inductor. Doesn't this mean that when the resistor part is created in Altium schematic library, its value will be fixed at that time? This is because if we change the resistor value in the schematic, the actual manufacturer manufacturer part number will become different and will need to be changed, thus it will be simpler to just have a separate part for each different value resistor. Correct? \$\endgroup\$
    – quantum231
    May 15, 2023 at 14:03
  • \$\begingroup\$ I was working by myself, so found it most convenient to choose manufacturer/part number after doing the PC layout, so didn't want that info embedded in the schematic. In a more controlled environment, where you can only used company-approved parts and suppliers, it may make sense to embed the manufacturer/part number info in the schematic symbol. \$\endgroup\$ May 15, 2023 at 15:30
  • \$\begingroup\$ So what you mean is that, the schematic uses a generic resistor symbol and has corresponding package like 0602 e.t.c. Then, before you place order, you assign a part number in the BOM? Is the method to make this flow work correctly defined anywhere? \$\endgroup\$
    – quantum231
    May 15, 2023 at 15:48
  • 1
    \$\begingroup\$ As I said, I was essentially working by myself, and made sure that I ordered the parts I required. The organization I worked for had no organized procedures for the PCB design process - there were several independent departments that each did their own thing. \$\endgroup\$ May 15, 2023 at 18:39

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.