I have as issue where rectangular pattern is not working as it should be.
screen cast attached
model: https://a360.co/2UbAAUn
Extrude cut with pattern BUG
Hi Gregor - OK. It took me some time to see exactly what is going on here. I cannot say for certain if this is indeed a bug - but the behavior of the software is difficult to follow. I will check it with some of the development teams.
However - it is not really difficult to see why there may be undesirable behavior from the software, as the structure of your design is not ideal.
The root of the issue is that you have created two components: "Component 1" and also "Mid". The outer edge of the box has NOT been defined as a component.....this is simply a Body - under the name "Base". In the first pattern of your cut - the cutting is occurring in both the component "Component" and also in the body "base". Once you switch to the variant with the component "Mid" - the same cut is trying to cut two components, namely "component" and "mid".....I am not sure if the software is SUPPOSED to do this, or not....there may be a limitation - or perhaps I am forgetting something. In any case - I can certainly understand how a user would be confused by this. I will discuss it - as already stated.
I would, however, make another suggestion, which I believe will result in 1) solving your problem 2) better, more reproducible results for all cases in the future.
Is there a particular reason this assembly structure was chosen? I cannot see an obvious reason to create the base body as a body in Fusion, while creating the two other bodies as separate components. Additionally - the two components have been defined by creating sketches which are embedded in the components themselves, and not at the top-level of the assembly.
The structure effectively creates sketches which are defined in one component, and uses these to define features in another component. In most other CAD systems, this would not be possible at all without the use of an assembly feature - and even then - these are notoriously unstable and very bad for performance. In truth - it looks like we don't handle it all that well either in this case.
I would suggest instead to either choose a top-down design structure (clearly the better choice in this case) or a bottom-up structure and remain consistent in their use, instead of doing both - as was the case here. It is much more likely to cause trouble for the software - but also - and this is even more important, it will be very difficult to follow your design. Changes will be difficult, and reuse will be impossible. In effect you get the worst drawbacks of both philosophies - with none of the advantages.
Here is a link to my Version for you: https://a360.co/2OxtbcC
and here is a link to a YouTube video I made on top-down design: https://youtu.be/L9Evb3ZxD40
and here is a link to a video where I discuss your file and the version I made: https://www.youtube.com/watch?v=hdIWHIMtbiw
I hope it helps you. I will respond again after speaking to development.
Mickey Wakefield
Fusion 360 Community Manager
Thank you Mickey for looking into this. Yes design is not ideal, was just one quick and dirty box just to demonstrate.
So I made another design (for example book shelf) that i think is best for my type of work (correct me if I'm wrong)
Its similar design and now the shelf component is touching middle component and has holes in it.
If i change my mind and i don't want middle plate, i want to remove or delete middle component, extend shelf to the right plate,... The result at the end is still the same. If i want holes where is want then, i need to delete pattern and make new one, so IMO its still bug. (log has been place already FUS-48841 )
I hope its now clearer.
thank you
Hi -
OK - so this time, you created all of the parts using bottom-up design philosophy. That is better - but at the very end you still created a sketch for the holes which are PART of the component "shelf"......the issue I described in my earlier post has not changed.
This would not function at all in a traditional CAD package. There is no direct way to create a hole sketch in one part and have it cut into another. (There are some ways available to create a sketch at the assembly level and have them cut into the individual parts - but this is not what is happening here. Here - we are creating a sketch in one part - and expecting this sketch to cut in another. That is a no-go.)
You CAN solve the issue easily and quickly though by using top-down design as I described in my video. There is no need to create each part individually and place their defining sketches inside of them. Top-Down design will give you the flexibility you desire and it will make this work - in ALL CAD systems!
Alternatively - you COULD keep making your components FIRST as you have - but then you need to make sure that the final sketch, (the one with the holes) is NOT part of one of the components. THAT sketch must be at the root level of the assembly. In this way - it will be possible to make your feature work - but ONLY if there are NO references to the parts themselves. This means, you cannot place your top-level sketch on one of the components' surfaces! This would create a REFERENCE to that part, which would again cause potential conflict. Instead - you will need to create a reference plane at the root level of the assembly which does not reference ANYTHING in the parts. In this way - you will effectively be creating what is called an assembly-level feature in other CAD systems that are based on the bottom-up design paradigm. While this CAN work - I can tell you from several decades of experience that they are generally a bad idea due to poor performance, instability and the fact that they create references between parts which make them unusable in other assemblies.
This type is feature is PRECISELY why Top-Down is the preferred design paradigm for this kind of assembly. It will allow you to change EVERYTHING in the assembly - and everything will still fit - the features will all work and the whole thing is manufacturable!
Mickey Wakefield
Fusion 360 Community Manager
Accepted solution
Hi Gregor -
Your other duplicate post (https://forums.autodesk.com/t5/fusion-360-support/extrude-cut-with-pattern-bug/td-p/8692754) has indeed been evaluated and deemed to be a defect. Please be aware that this does not mean we will immediately fix this issue - it means only that it has been noted, and that our development teams will possibly add it to their development sprints in the future.
I would still advise you strongly to use a consistent modelling strategy as I have already discussed. This will achieve consistent results - not only with Fusion 360, but with other systems as well and it follows common structures such that others will be able to understand and use your models. It will make your work much easier as well.
Also - my guess is that very few people will experience this defect, as it only occurs when modelling in a way that is non-standard. This means it is unlikely to be a high priority to fix. It may be some time before this is corrected.
I do hope I am wrong - but I would like to advise you as well as possible for you to be able to achieve your goals.
Mickey Wakefield
Fusion 360 Community Manager
