Updated files :
TSYS01.fzpz (23.3 KB)
Updated files :
TSYS01.fzpz (23.3 KB)
Schematic view connection terminals not propperly defined:
They should have conection on the tip.
The problem is that you defined Width 0 in connection terminals
You should change from this:
to get this:
1234 1234 also makes no sense, we added the actual pin functions now
The terminalIds are actually a 0.9.6 bug. A zero width terminalId used to work (and parts factory generates them on the generic IC!) This is 0.9.3b with a generic IC dragged in to schematic and connected to a header. Aligned correctly.
this is 0.9.6 with the same input. TerminalId not recognized. I will report this as a bug.
As well at least the SHT35-D.fzpz (I didn’t check the others) has no breadboard layerId which will prevent the part from exporting as an image (png, jpg, pdf, svg)
Thank you for the update,
have you seen my updated version on top of this post ?
it should work on all versions of Fritzing
the ID’s of the connections are now present in the svg which is imported in the part editor and therefore present in the component library file.
I have now. I fixed up the sht35-D part to meet the graphics standards like this (the others likely need the same) note I am using Inkscape here rather than Coraldraw so some things may be different for you. If you can figure out how to do the equivalent thing in Coraldraw the documentation would be appreciated to add to the tutorials section of the forum!
slightly offset (not enough to matter likely) in starting coords
so ungroup rescale and regroup and name the group breadboard. Rescaling in Inkscape is described here:
don’t know how to do this in Coraldraw or Illustrator (not sure it is possible in Illustrator!) Which produces this:
which is pretty much identical except meets the standards which are available here:
part file format:
and the graphic standards
While this will work, it isn’t the correct scale and doesn’t meet the graphics standards and thus I chose to replace it with the template file which looks like this
which is available here:
Since this is a sensor and by convension in puts are on the left of schematic delete the left, top and bottom connectors then duplicate the other 3 connectors, add their labels and pin Ids to give the final schematic that meets graphic standard.
Incorrect scale, silkscreen color is white (old style) rather than black (current style) and copper layers are above silkscreen (which makes Fritzing select the silkscreen first which is undesirable.) So ungroup rescale and change silkscreen color from white to black. Then for each pin, set the radius to 29 and the stroke-width to 20 to produce a 0.038000 hole for a 0.1in header.
to produce the final pcb svg
fzp file (edited with a text editor rather than parts editor which I find mostly useless)
add a fritizng version number
<?xml version='1.0' encoding='UTF-8' standalone='no'?> <module referenceFile="generic_sip_5_300mil.fzp" moduleId="SHT35-D_e71e8b6b9db09637b65141a2f76971d9_2" fritzingVersion="0.9.6">
Change the label to M (for module)
add proper tags
<tag>SHT35-D</tag> <tag>digital humidity sensor</tag> <tag>sensor</tag> <tag>fritzing user</tag>
change family to
<property name="family">SHT35-D</property> <property name="variant">1</property>
as it is likely unique. The family should only be the same for parts that can be swapped for each other (although that is not true for all the parts in core, it should eventually be made to be that way.)
added a url pointing to the github code repository (which has pictures of the board so the user knows what they are looking to buy, I didn’t find many sales sites.)
replaced the icon svg with the breadboard svg to save some file space.
ran the fzp file (and thus all the svgs) through FritzingCheckPart.py to fix up all the things Inkscape does which Fritzing does not support and to check for errors (such as missing layerIds)
$ FritzingCheckPart.py part.SHT35-D_e71e8b6b9db09637b65141a2f76971d9_2.fzp
Use 7zip to zip the resulting files in to an fzpz file then load the result in to Fritzing for testing. That immediately shows up an error, in schematic I reversed pins 1 and 2 (connector0 and 1):
so go back and correct that!
It now looks correct
note the entire .1in of the pin is green (or red if it is not connected) here and the terminalId insures the wire connects to the end of the pin.
run DRC (Routing->Design Rules Check) to verify it is OK.
move a couple of traces to the top layer to make sure traces on both sides work (this won’t find all possible errors but covers most of them!) Then export the pcb as gerber files and check the gerber output is correct. Firt edit the drill.txt file with a text editor and verify the holes are all 0.038in:
; NON-PLATED HOLES START AT T1
; THROUGH (PLATED) HOLES START AT T100
the 0.038000 in T100C0.038000 indicates the hole size in inches.
then view the board in a gerber viewer to make sure the translation took place correctly (this occurs after pcb view in Fritzing so problems that won’t show up in Fritzing are possible here.)
then suppress copper layers to leave only the drill holes to make sure all holes expected have been drilled.
which results in this corrected part (which has the same moduleId and files as the original, so you will need to delete that part before being able to load this one!)
SHT35-D-improved.fzpz (17.6 KB)
hope this helps!
A question for vanepp regarding graphic standards.
BTW thaks for it as I didn’t know that they existed.
I dowloaded the template file and found something in SVGs. What are these empty layers inside pcb SVG for? :
Should I guess you can customize part cutouts and soldermask?
I think future growth. I’m not aware of any way to use them although there may be.