Fusion
You might want to try using External Components (linked) in your assembly. Then when you need to replace one you can use the Replace Component command. This command only works on external components but it normally maintains all Joints, that are relevant, without issue. You have to be smart on the use of Joints so things can be replaced without issue.
You also might consider Configurations, if you have a Subscription License.
John Hackney, Retired
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Joints can use features that do not change between component changes, in my video I use the case radii to apply the Joint, this will probably not change in my design where the bolt holes will.
You need to gather up one of your assembly models and attach it so the Forum users can determine your modeling style. You need to explain a few of the problems, in this assembly, to direct those responding to your modeling methods and possible changes. We blind to your modeling methods. If you do not know how to attach your Fusion 360 model follow these easy steps. Open the model in Fusion 360, select the File menu, then Export and save as a F3D or F3Z file to your hard drive. Then use the Attachments section, of a forum post, to attach it.
John Hackney, Retired
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If you are using linked components and they are still being changed, why is there a need to use the replace component?
When the change to the linked component is changed, you'll get an update notification and simply update the assembly design.
Things still may break, but that is simply the result of changing inputs to references.
I don't replace the component--should have said updated to the latest version.
My comments about having to do the rigid group were when the original component was first referenced. That rigid group always breaks when I update to the latest.
Same with projected geometries and many extrusions.
One of the key purposes of doing the the 3d models is to make sure connectors align in three dimensions. When they don't, I have to tweak the layout of a pcb, reload the model and update the top level model to see if the change fixed the issue.
Also, iterating on connectors based on availability. Substitutes are never exact mechanically. Insulation height, pin lengths, etc.
Doing the fix takes a couple of minutes. Fixing the model takes too long. Hence, the workaround by adding the latest version of the component and keeping the stale one there. Works, but I think it will become unmangeable.
As I'm going through the side by side (updated reference versus non update) comparison of the timeline operations I'm keeping track of all the issues. Here's a typical one:
I figured out what joint failed by looking at the timeline of the model before doing the update. It was a joint between connectors. One connector is a sub-component of the external component that was updated to the latest version. The other connector is a also a subcomponent of another model that is externally referenced.
But, I have no way to know that without going back to the model without the updated reference. I just do a new joint and delete the original (there's no way to repair the original joint, as far as I can tell.
Here's what the timeline looks like after refreshing the linked component:
I've gone through the repair process several times. Once I've figured out what each operation actual was, it didn't take long to fix. First time was almost a full day to repair. Now I can do it in a half hour. But, I'm going with the work-around unless I get a better suggestion.
"I don't replace the component--should have said updated to the latest version"
Important distinction, certainly. But, knowing this helps. In general, you should not see a huge number of failures from a simple edit/update cycle. However, that will depend a lot on what goes into the edit process. So, a question:
- what kinds of edits are you doing in these cycles? If you are getting this level of failure, you must be doing a LOT of editing. Can you explain what sort of edits are going on?
I have some recommendations for what to do/not to do to minimize this. So, rather than try to to help you fix the errors, I'd rather try to help you prevent the errors in the first place.
@Phil.E and I did a class at Autodesk University in 2020 that included some of these tips: Debugging-Your-Fusion-Design-Lets-Get-Rid-Red-and-Yellow-Features . There is a video there, and the presentation and handout are also available. It's an hour class, but only part of it focuses on this topic. Of course, it is all valuable, IMO, but some areas less so for your question. The relevant sections start around slide 16. Some of the content here is intended to help you understand how geometric references are tracked and resolved. Knowing that will help you make changes that will be less likely to cause downstream failures.
The number 1 rule, though is: Always edit, never delete. This gets back to how Fusion (or any CAD system - they all use the same basic mechanism) tracks these references. Geometries all have some kind of identity. Bodies have a body name, Sketch curves have just an integer that is assigned to them. Components have a "path" through the hierarchy to help us determine which instance of a component you are referencing (it does matter). Body geometry is identified with a set of data that can include the identity of its predecessor geometry. So, for instance, if you draw a triangle, each sketch line will have an ID. If you extrude that triangle into a prism, each side face of the the prism will have an ID that says "this face came from sketch line X, and was created from extrude Y". If you then fillet an edge of the prism, that fillet face will have an ID that comes from the edge being filleted (which references the two adjacent faces' IDs), and also includes the ID of the fillet feature. So on, and so on. So, say you want to make the triangle longer in the extrude direction. You could delete the extrude and create a new one. But, since the ID of the extrude is part of the identity of every face of the prism, those faces will all have brand new IDs. So, any reference to those faces will fail. Similarly, if you want to edit the triangle, you can edit the sketch. You could delete one of the lines, and replace it with a longer one. But, again, the IDs of faces are based on the IDs of sketch objects. You've created a new one, so all faces from that line will have new IDs. Instead, if your sketch has dimensions, you can make the triangle longer by just editing the dimension instead of deleting and re-creating parts of it.
That's just one example, there are others. So, maybe if we understand your workflow better, we can help you prevent seeing these errors (or at least see fewer of them) with some improvements to those workflows.
Hope this helps
Jeff Strater
Engineering Director
Have you considered changing from KiCad to Fusion Electronics?
In theory, that could make things easier.
If you have looked into it and even tried, how was your experience?
@davethomaspilot9V8SL wrote:
I'm not willing to invest the time required to get skilled in a new set of PCB design tools.
Over the decades I've probably used a dozen and got skilled in a few. It takes a while to really get proficient in using the tools. Beyond having to always look up how to do this or that.
Agreed, I was initially not trying to convince you to learn another PCB tool. In case you had tried it, I was interested in how it "felt".
@davethomaspilot9V8SL wrote:
....
Really, I use Eagle for schematic entry and pcb design. I mostly just use Kicad to get the step files. I import the Eagle project into Kicad, then export a step file.
At this point is where I would recommend to look into Fusion 360 electronics. First, eagle is not being developed anymore and all the development efforts go into Fusion 360 electronics. At some point in time Eagle will be phased out! As you already are using Eagle, the transition should mostly be smooth.
The integration into Fusion 360, if it doesn't completely eliminate the amount of rework you have to do after changes to the PCB, then it will substantially reduce it!
"The typical thing I do is to create a step file for a pcb in Kicad. Then, I upload that step filel into F360 to create a component"
"If I change the pcb mechanically (different connector or board outline , for example) I create another step file (as I mentioned above)."
OK, more good information. That is a much different workflow than I assumed. I assumed that you were editing the referenced component yourself, in Fusion. So, a lot of what I said above is not applicable. If you are re-generating a new STEP file each time, there is a good chance that all of the geometry IDs will be wrong. It depends a lot on how Kicad generates the STEP file.
Also, how are you using the updated STEP file? Are you using "Upload new version" from the data panel? I'm not sure exactly what that will do, but it might help (as opposed to merely translating the new STEP file, inserting it, and deleting the old one.
There is also a capability in Fusion called "AnyCAD": How-to-use-AnyCAD-functionality-in-Fusion-360 . The purpose of this system is to precent the exact kinds of failure you are seeing. I know it works better with parametric file formats such as Solidworks, but there is at least an attempt to try to prevent reference failures that might be worth checking out. I have never used this, so I can't really help you, but the documentation should point you in the right direction.
If none of that works, then there is nothing to really do but the hard work of repairing all the references, just like you are doing, sorry.
I guess the one thing you can do is to minimize your geometry reference, and to use the most stable and largest-grain references you can. For instance, a face reference is more stable than an edge reference. And, a body reference is more stable than a face reference, etc. You can't always do that, but it is worth trying. Also, only project what you need - I've seen lots of designs that over-project edges in sketching. Turn off "Auto project edges on reference", because that can generate tons of unneeded and inintended projections without you even knowing it.
Jeff Strater
Engineering Director
