Incorrect component models in 3D viewer?

niari · July 10, 2017, 11:14am

I have found the 3D viewer quite useful. On my first board it saved me from having 3 terminal block connectors the wrong way round.

It’s worked fine for my last 3 boards apart from some components not appearing to have 3D models.

My latest board though bares no resemblance the footprints in the board layout.

Some of the capacitors are way way bigger than their footprints.

So, incorrect models for these capacitors?

Thanks.

Rene_Poschl · July 10, 2017, 11:20am

You need to update the 3d models. Download them directly from github.

The problem is that there are now correctly scaled 3d models. Therefore the footprints have been changed to have scaling 1,1,1.

Another problem is that footprints are downloaded directly from github without control by the user. Whereas symbols and 3d models are not updated at all. (This results in inconsistent libs for the users.)

I would suggest to switch to a local footprint lib setup where you use the footprint lib setup. Either by following the tutorial by @bobc:

Or by using the footprint lib downloader python script found in the kicad-library-utils repo.

github.com

KiCad/kicad-library-utils/blob/master/download_pretty_libs.py

#!/usr/bin/env python
# -*- coding: utf-8 -*-
#
# Download script for KiCad version 4 libraries. 
# KiCad version 5 does not need such a script as all footprint libs 
# are consolitated into one repository (https://github.com/KiCad/kicad-footprints)

from __future__ import print_function

import argparse
import sys
import re
import os
import subprocess
import platform

# Github address information
GITHUB_URL = "https://www.github.com/KiCad"
GITHUB_URL_SSH = "git@github.com:KiCad"
GITHUB_FP_LIB_TABLE = "https://raw.githubusercontent.com/KiCad/kicad-library/master/template/fp-lib-table.for-github"

This file has been truncated. show original

niari · July 10, 2017, 12:57pm

Thanks for the response. I followed the instructions “How to install local Footprint libraries”, closed Kicad and re-opened it.

The 3D view remains the same.

Rene_Poschl · July 10, 2017, 1:01pm

You still need to update the 3d models. The local footprint libs only help against future problems.

Rene_Poschl · July 10, 2017, 1:17pm

git clone?
or download the complete repo as zip?
Put them wherever you want just make sure KISYS3DMOD points at your downloaded files.

niari · July 10, 2017, 1:18pm

Do I use Preferences > 3D Shapes Libraries Downloader?

Rene_Poschl · July 10, 2017, 1:19pm

That’s even better. (I did not know you are on nightly.)

niari · July 10, 2017, 1:19pm

I’m not. Downloading now.

niari · July 10, 2017, 2:19pm

Thanks. Downloaded and working now.

niari · July 10, 2017, 2:43pm

Although not quite perfect. All capacitors on my original board are now correct including the electrolytics. However on my earlier boards they aren’t. Many of the electrolytics are too small.

I’ll play around more tomorrow.

Rene_Poschl · July 10, 2017, 2:56pm

The footprints on your old board now need updating. (Once a footprint is placed on a board, it is copied into the header of the pcb file. Changing it in the lib does not update the original pcb.)
Another option is to have the old 3d files somewhere and change KISYS3DMOD to point to them when you few a old project. (If you cloned the git repo simply checkout the correct tag/release)

niari · July 11, 2017, 12:06am

Thanks. So how do I update the footprints in my 3 existing projects?

The capacitor in this one was correct before I downloaded the updated 3D models.

Joan_Sparky · July 11, 2017, 12:34am

right click on ANY footprint in your layout, choose ‘Edit Parameters’
then hit the [Change Footprint] button
in the new dialog under ‘Options’ select ‘Update all footprints on the board’ and then hit [Apply]

… in case that fails…

open EESchema, re-create the netlist (export)
then back to PCBnew and import the netlist again, select ‘Exchange Footprint’ option ‘Change’ instead of ‘Keep’

niari · July 11, 2017, 4:06am

Thanks. Option 1 did the trick. On one of my boards updating the footprints completely moved a relay but I that was easily fixed.

Rene_Poschl · July 11, 2017, 8:44am

It also moves all reference designators and values back to their original position. You might need to recheck that no silk reference is now covered by a nearby component or a via.

niari · July 11, 2017, 8:58am

Thanks very much. Already noticed and done that.

Joan_Sparky · July 26, 2017, 10:52am

ChrisGammell · July 27, 2017, 11:53pm

ChrisGammell · July 27, 2017, 11:54pm

forthnight · July 28, 2017, 9:16am

Often when the components are of incorrect size, the scaling issue is due to SI vs imperial units. That is, that the 1.0000 scaling should be divided by 2.54 (one inch is 2.54 cm): 1.0000 --> 0.3937007874…

However, this is against KiCad library convention, stating that good practice is using scaling 1.00 in all directions.

The by far easiest fix is to install FreeCad and add a macro
which is designed to make life easier when working with footprints and 3D-components in KiCad. The macro is called “KiCad StepUp”, and adds a bunch of tools to FreeCad, including automatic rescaling and so forth. It also makes much better renders (photo realistic).

Grab it here: https://sourceforge.net/projects/kicadstepup/

Image showing FreeCad with the StepUp tools to the right of the capacitor. You can import mod-files, pcb-files, etc and export to STEP and WRML (with automatic rescaling and color selection to different parts).

It is also easy to move components to make them fit the footprints. This is a pain in the ass in KiCad.

(This post was originally much longer with more pictures and relevant links, but because I am a new user here, I was not allowed to post it as there is a limit of 1 pic and 2 links…)