Fusion 360 complex models, assemblies and component misalignment

[TorontoBuilder]

Okay I have a confession to make. When I design in fusion 360 I dont use the typical modeling method of modeling parts around an origin and then moving components into an assembly under the assemble tab.

My technique is a legacy from when I was learning and I would model up bodies only, and then orient each body in relation to a fixed origin point. Bad technique I know but I'm slowly trying to change how I model. I now make components and sub components, but I reference them to a fixed origin. I need to slowly change and start using the assembly tab to make assemblies.

One side effect is that I sometimes inadvertently drag a component or body out of alignment, and can't find where I messed up...

So a question, to anyone who uses fusion assemblies, can you create components and then assemble, and then create new components and assemble further, and once you have done so does it lock in your components so you can't inadvertently drag something out of alignment?

 

[PeterT]

I'll let the F360 users comment on specifics, but 'generically' in 3D CAD you want to be comfortable both ways as dictated by 'best practice' which is kind of specific to the project. I'm about to use SW vernacular but here goes with examples

Bottom up assembly. Each part is drawn as a single entity. A piston is a 'part'. Same goes for a ring, a con rod.... They come together in an assembly called 'engine' entirely defined by mates. This part is concentric to that feature/part. This part is co-planar to that feature/part. This rotates about that etc. There are nuances. I could have 25 different configurations of piston, all within the same piston part file. But depending on which one is toggled, the assembly just reloads & refreshes so long as the defining mates are still relevant. This gives tremendous power of permutations & combinations. There is another concept called sub-assembly. Kind of like, bring in the whole transmission assembly to my engine powertrain assembly, but load it in a manner that not all 5000 transmission parts & their mates are 'live' (which makes for lots of CPU processing). The takeaway here is design wise is bottom up mode, you would not start with a crankcase & then develop all the other parts 'from' that part. Its basically too complex, cons quickly outweigh pros. This gets into data management because the assembly has to be aware of all the parts in terms of their data path, configuration, material.... Delete or rename a part, the link potentially becomes broken.

Top own assembly. Kind of the opposite of above. You start with a 'something' call it a base part & then other parts are inherently related to this part. I start with a dresser box 48" wide & design 5 drawers with clearance & hardware. I change the dresser to 42" wide & like magic all the drawers compensate. This is powerful too but in a different way.

So 'origin' (at least in SW) doesn't really have much meaning. A part should always have an origin. But once the parts is imported into an assembly, the mates take on a higher priority status & the part origin will be wherever it will be. Its still there & somewhat useful, but it was only kind of necessary to develop the part.

Then enter workflows like 'weldments', kind of a sub module. With some very simple construction lines you can define a complex structure in 3D space. Then basically start defining this stick is tube Type-A. That stick is Type-B. As you proceed select from a host of end treatments & it does all the notching & allowances & spit out a cut list of all the constituent parts. (Notice this kind of like mates but not really mates). This is different to above workflows, but just mentioning as an aside.

Hope this helps. I realize I'm speaking a different cad dialect but from what little I've seen of other modelers, they are kind of similar.

 

[eotrfish]

I haven't played with Fusion for years. It was originally provided as a bonus with Inventor Professional. If it is anything like big brother Inventor there should be constraints that can be applied to the parts. The first part in an assembly can be grounded - usually to the X_Y plane. Subsequent parts can be constrained to part #1 - or to each other, and then just one of them constrained to part #1.

 

[TorontoBuilder]

I'll let the F360 users comment on specifics, but 'generically' in 3D CAD you want to be comfortable both ways as dictated by 'best practice' which is kind of specific to the project. I'm about to use SW vernacular but here goes with examples

Bottom up assembly. Each part is drawn as a single entity. A piston is a 'part'. Same goes for a ring, a con rod.... They come together in an assembly called 'engine' entirely defined by mates. This part is concentric to that feature/part. This part is co-planar to that feature/part. This rotates about that etc. There are nuances. I could have 25 different configurations of piston, all within the same piston part file. But depending on which one is toggled, the assembly just reloads & refreshes so long as the defining mates are still relevant. This gives tremendous power of permutations & combinations. There is another concept called sub-assembly. Kind of like, bring in the whole transmission assembly to my engine powertrain assembly, but load it in a manner that not all 5000 transmission parts & their mates are 'live' (which makes for lots of CPU processing). The takeaway here is design wise is bottom up mode, you would not start with a crankcase & then develop all the other parts 'from' that part. Its basically too complex, cons quickly outweigh pros. This gets into data management because the assembly has to be aware of all the parts in terms of their data path, configuration, material.... Delete or rename a part, the link potentially becomes broken.

Top own assembly. Kind of the opposite of above. You start with a 'something' call it a base part & then other parts are inherently related to this part. I start with a dresser box 48" wide & design 5 drawers with clearance & hardware. I change the dresser to 42" wide & like magic all the drawers compensate. This is powerful too but in a different way.

So 'origin' (at least in SW) doesn't really have much meaning. A part should always have an origin. But once the parts is imported into an assembly, the mates take on a higher priority status & the part origin will be wherever it will be. Its still there & somewhat useful, but it was only kind of necessary to develop the part.

Then enter workflows like 'weldments', kind of a sub module. With some very simple construction lines you can define a complex structure in 3D space. Then basically start defining this stick is tube Type-A. That stick is Type-B. As you proceed select from a host of end treatments & it does all the notching & allowances & spit out a cut list of all the constituent parts. (Notice this kind of like mates but not really mates). This is different to above workflows, but just mentioning as an aside.

Hope this helps. I realize I'm speaking a different cad dialect but from what little I've seen of other modelers, they are kind of similar.

I use the top down assembly, and the project I'm working on now is a new kitchen from scratch designing each frameless cabinet, drawers, doors, hinges etc. I started with a reference plan view, and then used the origin of that view to create 3 elevation sketches of the cabinets from which I extruded the main cabinet panels. I did this to assure that I dont have any surprises when I get the cabinets back home and try to actually install them.

But something got shifted. I think I could have just drawn each cabinet and then assembled using base sketch with a few critical reference points.

 

[Arbutus]

I have been using Fusion since it's inception.

For folks who are "migrating" to F360 from something else, my primary advice is FORGET EVERYTHING - START OVER

Solid objects in F360 start with a sketch. A sketch can exist on any plane. Sketch profiles are used to extrude, cut and intersect. When extruded, the sketch creates a body. The solid BODY is an arbitrary 3D object which cannot be assembled with another BODY, but it can be further combined, cut, and extruded to complete the geometry. I think of BODIES as lego bricks which you can design to meet any rational geometry and then assemble as needed.

When you are ready to make an ASSEMBLY, the bodies must be converted to COMPONENTS. When you copy a McMaster Carr item into the project, that is a COMPONENT too. Now you have components you designed, or components someone else designed. COMPONENTS are joined with constraints called JOINTS, which are referenced to the COMPONENT ORIGIN.

Most F360 novices do not plan their designs. Fact. Those designs are unstructured, like a disk drive without folders, just files. That makes it very difficult to find, adjust and replace parts.

The correct workflow is to create a new design, create a parent component and then as a child of that component create a new (empty) component for each major sub assembly. Each sub assembly can be built from one, two or ten thousand components, with the JOINTS between each defined.

When the sub assemblies are completed, the parent component is fully described.

A change to an underlying SKETCH changes its associated BODY which updates the affected COMPONENTS and therefore the parent. This is how F360 (and other systems) use parametric data to generate any number of components from one model.

When the edges, points, faces, holes, etc which are used by a JOINT are edited, by deleting something in the sketch or body, the joint becomes dereferenced and the COMPONENT fails. Similarly, if two bodies are positioned together (not JOINED) and one is moved later, any parts using that geometry will fail.

So I strongly suggest that the top-down component - subassembly workflow is followed. There is no quick fix for a messed up model unless you backtrack the history and figure out where you went wrong. Starting the project properly is the best way to avoid frustration.

-------

For members with a good Zoom connection (sorry @Susquatch ) if there is interest, I would be willing to host a Fusion 101, 102 and 103 on-line class covering the basics.



Don

 

[Susquatch]

For folks who are "migrating" to F360 from something else, my primary advice is FORGET EVERYTHING - START OVER

Prolly excellent advice but in practice VERY difficult to follow.

For members with a good Zoom connection (sorry @Susquatch ) if there is interest, I would be willing to host a Fusion 101, 102 and 103 on-line class covering the basics.

For a little while there it was looking good for a fibre connection. It fell apart when they looked at what was really required. A very bad project executed by idiots. Long story short, it's not likely gunna happen anytime soon. So I'm still not zoomable.

 

[Mike R]

I thought I was getting proficient in Fusion, but for whatever reason, many models I built that have lots of parts are now a scattered mess. Its like one of the updates blew up the mates and now the parts are just randomly scattered. This is on multiple projects.

Now I'm probably the actual guilty party for 90%, going in and modifying a sub component and breaking its mate, but I definitely feel it wasn't all me....

So I've given up drawing large assemblies in Fusion unless absolutely needed (i.e. my own design) for the time being. This goes along with the desire to find an alternative to Fusion...another story.
Example broken models here:

 

[Upnorth]

Okay I have a confession to make. When I design in fusion 360 I dont use the typical modeling method of modeling parts around an origin and then moving components into an assembly under the assemble tab.

My technique is a legacy from when I was learning and I would model up bodies only, and then orient each body in relation to a fixed origin point. Bad technique I know but I'm slowly trying to change how I model. I now make components and sub components, but I reference them to a fixed origin. I need to slowly change and start using the assembly tab to make assemblies.

One side effect is that I sometimes inadvertently drag a component or body out of alignment, and can't find where I messed up...

So a question, to anyone who uses fusion assemblies, can you create components and then assemble, and then create new components and assemble further, and once you have done so does it lock in your components so you can't inadvertently drag something out of alignment?

You should really watch a few youtube tutorials. It will make a big difference in your understanding. The advice Arbutus gave about forgetting everything and starting over is 100% correct. I switched from Solidworks to fusion and tried to use both for a while. I deleted Solidworks and just used fusion. You have many options in Fusion for joints. They can have motion or be rigid. Ridgid ones are probably what you want. They will be permanently fixed in position.

 

[TorontoBuilder]

You should really watch a few youtube tutorials. It will make a big difference in your understanding. The advice Arbutus gave about forgetting everything and starting over is 100% correct. I switched from Solidworks to fusion and tried to use both for a while. I deleted Solidworks and just used fusion. You have many options in Fusion for joints. They can have motion or be rigid. Ridgid ones are probably what you want. They will be permanently fixed in position.

Oh make no mistake, I have watched many tutorials from great teachers..

and I follow the top down approach and plan drawings in advance as arbutus says. But my issue is how I reference relative parts to organize an assembled project instead of assembling my components, unless I have a specific moving joint to test.

It's because I got into a bad habit I now need to change... because for decades I never had any assemblies in my 2d cad projects

 

[PeterT]

Broken links in a CAD modelers program can be problematic for sure. You have to be extra diligent because CAD tentacles extend even further into other nests. If I had a functioning engine assembly & decided to later rename Part 'piston' to 'piston1', the part itself doesn't really care. But the assembly only knows you referenced 'piston' in a Drive-X, Folder-Y, Subfolder-Z.... & now its not there, so tell me what to do. It has no way of knowing there was a change behind the scenes. But that is not a reason to model in a specific way (top down or bottom up). That's more about file management & housekeeping. Fundamentally not much different to my digital photo album originally contained a picture named Charlie. I renamed the jpeg to Charlie1 & now the album gives me a nasty message with a blank tile for what was Charlie.

Unrelated to assemblies, even the lowest denominator (SW Parts = Fusion Body?) typically have associated drawings & thus also links or associations between them. Parts can have names configurations so again if deleted or modified configuration, the assembly cannot be aware until it attempts to open the file upon loading. I could go on & on. This is such a big deal that SW used to have their own dedicated file explorer tool to sniff out instances & associations. Or Pack-N-Go that conglomerate all the constituent files wherever they are strewn across drives to transplant elsewhere. They have removed SW Explorer with a more rudimentary OS app which is too bad, but I suspect only because there is a much bigger 'industrial' data management module. When you start getting into thousands or millions of files being touched by many people, perpetually churning on changes & revisions - ya that's the big leagues.

 

[PeterT]

I deleted Solidworks and just used fusion. You have many options in Fusion for joints. They can have motion or be rigid. Ridgid ones are probably what you want. They will be permanently fixed in position.

I haven't run Fusion myself but I have a hard time believing SW is missing anything in terms of types & number of unique mates if that is Fusion speak for joints. I mean they are both perpetually evolving new mate features & shortcuts & this is only one small aspect of choosing one program over the other (cost being the elephant in the room). But now I'm curious since you have used both apps. What mate/joint capability or feature have you seen in Fusion that SW cannot do or maybe significantly worse at?

 

[TorontoBuilder]

So I just created assemblies from all my components and all the misalignments were resolved. It also allowed me to see the one component that was not referenced to the proper point.

My lesson is, to start with a base component, and create joints for assemblies as I create new components as a standard protocol

 

[Arbutus]

The parent component should only contain assemblies, components & joints. The subassembly components should also ONLY contain next level subassemblies, components and joints.

The component must be self-contained including it's bodies and sketches, other components (e.g fasteners) and it's internal joints. This allows the component to be externally referenced correctly.

The error I see from students most frequently is trying to JOIN components across the tree - that is quite wrong - it is the parent that owns the joints between it's children. If your component is active and you create a joint with another component, the joint relationship is contained in the first component. All is well, until you change that first component - now any other part that was dependent on the joints becomes dereferenced and you will see this as a misplaced object, or one that does not move together with the assembly when it is moved.

Select a component. Activate it. Now create a sketch, body, etc. Fully describe the component with its internal joints. Now select it's parent. With the parent activated, create your component-component joints. This generates a correct, hierarchal top-down model which allows individual components and subassemblies to be added, removed and duplicated without affecting the other parts of the model.

 

[Mike R]

Maybe I'm thick in the head, but I half understand this. I can see why it breaks, but not how you get around it.
Can you give a multi component or body example? I.e. I like engines - so usually I'm modeling a piston (cylindrical slider), rod (pin joint on 2 ends) and crankshaft (revolute) in a case (4 components). How should I structure and not link "across the tree" the piston to the rod, and then the rod to the crank? In my mind the case will be the parent of it all, and I've created the model of each of the crank, piston and rod. I can envision the joint for the piston to the case, and the crank to the case, (both to the "parent" so no issues) but what about the rod? Its joints are dependent on 2 other "children" (piston and crank). This is the one that get me.

 

[Upnorth]

I haven't run Fusion myself but I have a hard time believing SW is missing anything in terms of types & number of unique mates if that is Fusion speak for joints. I mean they are both perpetually evolving new mate features & shortcuts & this is only one small aspect of choosing one program over the other (cost being the elephant in the room). But now I'm curious since you have used both apps. What mate/joint capability or feature have you seen in Fusion that SW cannot do or maybe significantly worse at?

The only reason I switched to Fusion instead of using Solidworks was the price. I have an infinitely renewable Fusion license for $400 a year. I got rid of Solidworks a long time ago so can't really remember specifics about it now. The stuff I do isn't complicated enough to need any high end programming.

 

[Arbutus]

This is a simple design with three trays and an external reference to the mounting frame component.

Each tray is a separate component, self contained with a body derived from a sketch
The Mounting Frame component is a subassembly. This was a separate model which also contains two sketches and two bodies, converted to components, with the position of the left & right frames defined by a "rigid group" joint.

The parent component is the Tray Assembly. This is the currently active component (black dot after the component name) This contains 7 different trays (3 are visible) and one Mounting Frame. The joints called Rigid 1, 2 and 4. This is a complete, fully described model with the correct heirarchy.

The error I see most often is joints between components described inside one of those components - in this case say, Stacking Tray Medium Grid is JOINED to its neighbour Stacking Tray 8x1. All is well until Stacking Tray Medium Grid is deleted. Then the 8x1 tray will float away since the joint no longer exists. Therefore the joint between components must be described inside the parent of both components.

 

[Arbutus]

but what about the rod? Its joints are dependent on 2 other "children" (piston and crank).

Make a sub assembly with the pistons, cranks and rods:

Activate the top level component. Create a NEW empty component called piston assembly.

Add the pistons, rods and crankshaft which have been modelled either inside the design or an externally linked component.

Add the joint relationships. Test the motion using motion link.

The piston assembly is now a sub assembly in the Engine parent component.

 

[Mike R]

Thanks for that - I'll give it a try next time I try and model an engine - I have a small diesel engine idea in my head and need to get it out.

 

[Susquatch]

The error I see from students most frequently is trying to JOIN components across the tree - that is quite wrong - it is the parent that owns the joints between it's children.

You teach Fusion! Somehow I missed that previously.

What is your student base?

 

[Dan Dubeau]

Not sure how to explain it, but Fusion just never jived with my brain. I'm not a fan of how it handles assemblies, both locally and globally (I have the same gripes about solidworks and inventor too). I've used a few CADand CAM programs over the years, and they're all a bit different, but they all pretty much DO the same thing. I always equate them to driving a vehicle. They all get you from A-B, but with varying levels of sophistication and efficiency. Buttons and knobs might be different from brand to brand, but the basic functions are still there. Some just have extras. When learning to drive, it's important to focus on the foundational skills of driving an automobile, not "driving a chevy car" for example. Generally people can hop from vehicle to vehicle and get going relatively quickly with some quick familiarization of controls, but it might take a bit more time to learn all the finer points and features of each vehicle to fully exploit them. You might prefer one brand or another for whatever reasons. CAD/CAM software is the same thing. Focus on the foundational skills of learning to model, create sketches, constraints, dependencies, and assembly structures, and you can take that competency with you to various packages you may encounter. You may be used to driving an Mercedes (catia), and then have to make a quick trip in an old chevy corsica that stalls at every light (free cad) so you have to baby it to get where you're going, or drive it in a specific way so that it doesn't crash and the doors don't fall off because they lose their constraints and associations if you change routes on the way (fusion). I've always been pretty quick to pick up a new program with some poking and proding around, but Fusion, and Free cad sent me to the youtubes, and forced me to unlearn some habits to figure out how THEY wanted to be used instead. Call me set in my ways a bit, but I like having the options to work in different ways depending on the project at hand. You don't get that with cheap or free packages.....

Despite using fancy CAD for years, I still gravitate to dumb solids, old school surface modeling and 2d a lot with Rhino for most of my projects. I did a lot of that (surfacing) for work over the years, and still actually enjoy working that way. It's like the guys that prefer manual machining and cranking handles over CNC, I still enjoy old school CAD methods. That's not to say I don't use Parametrics and newer modeling techniques for some projects, they have their place for certain projects. Hainvg an autopopulating BOM is a must for some stuff. But for a lot of stuff, I'm still WAY faster the old school way. The problem comes when I've started a project the old school way, and it grows to where it should have been done in a parametric modeler, but I'm past the point of no return, so I just keep stubbornly driving on......(like my belt grinder project lol). I try to start projects in MD if I see a lot of iteration to get to the finish line, or if it's a large assembly that needs BOM control. For most projects that just need quick initial figuring and machining/fabricating it's Rhino.

I'm still a big fan of Mechanical Desktop and the way it handles modeling and assemblies, as it gives you so much freedom and different ways to do everything based on the task at hand. I weep for the day a windows update wipes out my ability to still use my 2006 version and I have to fully migrate to a new system. If that every happens I'll bite the bullet and buy Keycreator, as I've found it's the closest to MD in any new offerings, and really liked how it worked. Solidworks is fine too, but I wasn't as neurally compatible with it as I'd like. I'll never be without my Rhino though, it's like an extension of my brain at this point, as I've been using it for so long. If they just integrated parametric modeling like how MD did it, without changing anything else I would be a very happy man. Grasshoper while cool, is not the same, or same functionality as how i'd like.