Author Topic: Using same pattern for multiple components  (Read 3823 times)

0 Members and 1 Guest are viewing this topic.

Offline Thedon

  • Contributor
  • Posts: 6
  • Country: au
Using same pattern for multiple components
« on: November 03, 2016, 10:02:45 pm »
Hello all I have encountered a problem with my latest project. I’m trying to use a switch & potentiometer combined component to be specific a Bourns PTR901 the problem is I have created a pattern for the part and attached the pattern to the switch and potentiometer within the schematic. When I import the components into the PCB it creates two separate identical patterns so the workaround is to create two separate patterns one for the switch and the other for the pot and then overlap both patterns. The questions I have is this the only solution or can I create one pattern and attach the pattern to multiple components within the schematic? Also will my workaround create any issues when I export the gerber files? Thanks in advance
« Last Edit: November 03, 2016, 10:04:35 pm by Thedon »
 

Offline Farley

  • Regular Contributor
  • *
  • Posts: 84
  • Country: us
Re: Using same pattern for multiple components
« Reply #1 on: November 03, 2016, 10:58:06 pm »
What you are creating is referred to as a multi-part component. The multiple parts are defined in the Component Editor in DipTrace as a single component. That component is then assigned a single pattern from your pattern library.

See section 3.2.5 (Designing a multi-part component) in the DipTrace Tutorial PDF for a detailed explanation of how it's done.
http://www.diptrace.com/books/tutorial.pdf

The explanation begins at page 129.
 

Offline DerekG

  • Frequent Contributor
  • **
  • Posts: 822
  • Country: nf
Re: Using same pattern for multiple components
« Reply #2 on: November 03, 2016, 11:05:29 pm »
can I create one pattern and attach the pattern to multiple components within the schematic? Also will my workaround create any issues when I export the gerber files?

Yes, you can use an existing pattern (footprint) or design your own, then use that pattern many times over within the same schematic. An example of this would be the TO-220 footprint. This same footprint is used for voltage regulators, mosfets, IGBT etc, so is expected to be used many times over within the same design.

To attach a different footprint to a schematic symbol, double click on it & select "Footprint". You can then search your libraries for the footprint you require.
I also sat between Elvis & Bigfoot on the UFO.
 

Offline John Coloccia

  • Super Contributor
  • ***
  • Posts: 1199
  • Country: us
Re: Using same pattern for multiple components
« Reply #3 on: November 04, 2016, 04:50:30 am »
When you make you component, put the switch (for example) on the first page of the component editor, and then add a page, just like you would add a page to the schematic. Just right click on the tab at the bottom that says "Part 1", and click "Add". Voila. Put the pot on the second page. Now you have a 2 part component, and when you drag it into the schematic you'll get two separate parts.

Make your footprint to match the physical footprint of the pot/switch.

Now when you attach the component to the part in the component editor, you can select which pins of the component go to the physical pad on the footprint. It should be pretty obvious how to do it once you get over the conceptual hurdle of adding a page in the component editor to make a multiple component part.

This is extremely convenient. I do it all the time for things like Opamps, optos and other ICs that have multiple separate parts or sections inside them. For example, for a typical TL072 style OpAmp, I'll make 3 components: 2 opamps and a little block for power (V+/V-). Really helps neaten up the schematic.
 
The following users thanked this post: DerekG, Keicar, richardlawson1489

Offline DerekG

  • Frequent Contributor
  • **
  • Posts: 822
  • Country: nf
Re: Using same pattern for multiple components
« Reply #4 on: November 04, 2016, 10:12:48 am »
Now you have a 2 part component, and when you drag it into the schematic you'll get two separate parts.

John's advice above is excellent. It works very well.
I also sat between Elvis & Bigfoot on the UFO.
 

Offline Thedon

  • Contributor
  • Posts: 6
  • Country: au
Re: Using same pattern for multiple components
« Reply #5 on: November 04, 2016, 04:19:34 pm »
Thanks John excellent advice I was going about the wrong way by creating the pattern first and then attaching them to two separate existing components obviously the trick is to create a new component made up of the switch and pot, many thanks.
 

Offline John Coloccia

  • Super Contributor
  • ***
  • Posts: 1199
  • Country: us
Re: Using same pattern for multiple components
« Reply #6 on: November 04, 2016, 06:07:18 pm »
Thanks John excellent advice I was going about the wrong way by creating the pattern first and then attaching them to two separate existing components obviously the trick is to create a new component made up of the switch and pot, many thanks.

You're very welcome. :)
 

Offline technotronix

  • Regular Contributor
  • *
  • Posts: 209
  • Country: us
    • PCB Assembly
Re: Using same pattern for multiple components
« Reply #7 on: December 31, 2016, 09:45:18 pm »
Thanks for the useful solution john.
 

Offline richardlawson1489

  • Regular Contributor
  • *
  • Posts: 125
  • Country: us
    • PCB Assembly
Re: Using same pattern for multiple components
« Reply #8 on: January 20, 2017, 12:18:40 am »
When you make you component, put the switch (for example) on the first page of the component editor, and then add a page, just like you would add a page to the schematic. Just right click on the tab at the bottom that says "Part 1", and click "Add". Voila. Put the pot on the second page. Now you have a 2 part component, and when you drag it into the schematic you'll get two separate parts.

Make your footprint to match the physical footprint of the pot/switch.

Now when you attach the component to the part in the component editor, you can select which pins of the component go to the physical pad on the footprint. It should be pretty obvious how to do it once you get over the conceptual hurdle of adding a page in the component editor to make a multiple component part.

This is extremely convenient. I do it all the time for things like Opamps, optos and other ICs that have multiple separate parts or sections inside them. For example, for a typical TL072 style OpAmp, I'll make 3 components: 2 opamps and a little block for power (V+/V-). Really helps neaten up the schematic.

This is really an amazing solution. This is helpful for my next project.
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf