DWG/DXF export component position change

[derekmcleod]

I exported a Fusion file using the new DWG/DXF Export command in Fusion and the components contained within are in different positions when opened in Autocad. I tried a Rigid group in Fusion to lock everything in place and that didn't help. Same issue when exporting through A360 online. This is part of a lamp and the legs and body are rotated 90 from the intended position. The cord assembly is also shifted away. Any ideas? Fusion screenshotAutocad screenshot

[HughesTooling]

Can you share your Fusion f3d file? How are the parts positioned? Are they built inplace, if you've assembled them have you used joints? You might have problems if you have save positions in your timeline. If you can share the design can you share the DWG as well.

Mark

[derekmcleod]

I can't share since it is proprietary. There are two capture positions in the timeline but rolling it back doesn't show any changes. I created the legs as an extruded sketch in the intended position. The body was a revolved sketch but I did move it since it was created before the legs, although I didn't rotate it since it is round. I've been trying to work with components and having just one or two bodies contained within that are generated from sketches.   

[HughesTooling]

You need to follow Rule #1 for assemblies, pretty much one body per component. Never use move or save position on components, always build in place or position with a joint. I've never seen these problems building assemblies this way but I usually export STP files so there's a chance DWG and AutoCAD are the problem.

Try deleting all capture positions and moves and rebuild with joints. I guess you could try export as STP then reimport, if that works try exporting that file as a DWG.

Mark

[derekmcleod]

I've been following Rule 1 but occasionally move things around with the move command. It's hard to unlearn what seems like a simple/logical way to model things. I'll give it a try by deleting moves and capture positions. 

Why one body per component? There are two identical legs in my example, created as a single extrusion using two profiles drawn with the correct position in one sketch. Still trying to figure out best practices and these workflow ideas are not always the most obvious. 

[Phil.E]

Is there a pending capture position in your file when you export as DWG/DXF? If you see capture position waiting on the toolbar, this might affect export. 

[HughesTooling]

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@derekmcleod wrote:

Why one body per component? There are two identical legs in my example, created as a single extrusion using two profiles drawn with the correct position in one sketch. Still trying to figure out best practices and these workflow ideas are not always the most obvious. 

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For something simple I guess it's ok but still a bit of a bad habit. If you ever want to make 2d drawings the parts list would not be correct for example. Better to create one leg as a component then copy or pattern to create a copy of the component.

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I've been following Rule 1 but occasionally move things around with the move command. It's hard to unlearn what seems like a simple/logical way to model things. I'll give it a try by deleting moves and capture positions. 

I really don't like move in a parametric modeling program, there are parametric versions of move but most people don't seem to use them. A joint is far more useful, you can position and orientate with one feature and if you edit the part it's connected to the position will be maintained. Not sure why people struggle with move, I've seen designs on the forum where someone's used several moves to position a part and still not positioned accurately when one joint would do the job and the assembly would not fall apart with an edit.

Mark

[glitchform]

@HughesTooling This is very interesting. I am faced with the same problem as the OP. The assembly is all over the place when I export it as a DWG. It makes sense, after reading your reply, why this is happening. If I make the origins of all my components visible they are not aligned with one another since the components had been moved and rotated.

I will try to apply your Rule #1 to my workflow going forward, but I am struggling a but with selecting bodies that I want to move from the browser. If I turn every body into a component (to follow the "One body per component" rule) then what I end up with is having to drill down several levels just to get to the bodies in the browser. Shift-selecting becomes impossible. Also, how am I then to move several bodies at once, since I cannot move components? And what happens when I drag in a design from another file?

Or, a real example, I have a chain that contains 100 separate links. I can easily select and move them by moving the chain assembly that they belong to, but if I am not allowed to move the components or assemblies then I have to select the 100 bodies and move them. But what if I want to maintain the relationship of the chain links with some other part of the build that is outside of the chain assembly?

I am wondering why this rule is in place? It appears to me that I can rename the bodies and their names will display properly when I create a drawing. One component per body also creates a lot of origins to keep track of. It seems a bit more logical to me to group relevant bodies under one component. Not being able to create a group of bodies for easy selection makes the design process very tedious. Or am I missing something?

Could you please elaborate? I am new to this, and would like to know more about the fundamental rules. Thank you.

[HughesTooling]

Don't have the time to go into why components work for me.

Have a look at how easy this assembly is to manage, only 5 top level components.

Within these are more subassemblies, then each component contains the sketches that built it also note the timeline is in blocks where I create a component then all it's features. Easy for me to figure out what's going on and easier for Fusion to keep track and not end up slow and unstable. Maybe this workflow will not suit the way you work, you'll need to figure that out. With Rule #1 you make a component first and with it active create all the the features, you don't move bodies into a component. 

The 2d drawing workspace doesn't really work well with assemblies, it has no clue about the orientation of components, really there should be an option to create views based on the component origin not the document. In more traditional solid modelers you'd create each component\part in a separate file then create drawings from the files. Fusion using Components instead of files doesn't have any way of replicating the parts in separate files workflow for drawings. Brought it up a few times in posts but never got any answers on improvements.

Mark

[glitchform]

Thank you for your reply.

Your workflow makes perfect sense when creating parts from scratch. I also like how neat everything is.

I happen to work with a lot of loose parts that I drag into new files and then reassemble/rearrange, and the only way I found to do that quickly was to create and then move around components. It happens to work really well with STEP files and I never had any issues, but today I went to export a DWG and everything fell apart.

It looks like your workflow is definitely the correct way to do things, so I will try to see how I can incorporate it into my process. Thanks again!

[HughesTooling]

If you know you're likely to need to move a component around and use in other designs using copy\paste new you might want to experiment with positioning the component with a joint as soon as it created, then when moved all the sketches and the origin move together.

Here's an example in the same design.

Mark

Edit. Just to clarify, what I do is create the component, make its origin visible then apply a joint between the origin and a feature I want it joined to.

[derekmcleod]

Interesting discussion on this. 

Maybe related workflow question - how do you control where joints reside in the browser? In an older model I've made, the various components were made. When joints are used, they end up at the top level. When I copy/paste the jointed components (sub-assembly), the joints don't get copied, but at least I can make a rigid group. It seems like bad practice to move the components into a top level component after the fact, but I am not too sure. 

In a newer model, I made a top level component, then made sub-components within it, and the joints stayed inside the top level. This seems like a better approach. Copies have the joints within them as I hoped. When I joint the sub-assemblies however the joints are again at the top level. 

[HughesTooling]

Joints will be created in the component containing both components. So if you have one component in one subassembly and the other component in another subassembly the joint will be in whatever component contains\owns both subassemblies ( that could be the top level component, depends how many sublevels in component tree). 

If you can make a subassembly like you described containing all the joints and components it works quite well for mirroring components and maintaining joints as well.

In the example I show above where I created a component then straight away created the joint, it you use Copy/Paste New the joint in made into a save position. Personally don't like that, I'd rather the joint show a warning and ask you to reselect what you want it joined to. So I always roll the timeline to the save position, delete it and replace with a joint.

Mark