Having trouble with Fusion in general

[Anonymous]

So I'm having a bit of a workflow crisis with Fusion in general.

If I go top-down and just blast out stuff without a care in the world, it works out okay, but parametric relationships are terrible and none of the parts are drawn 'as manufactured.' This works out OK.

If I go 'bottom-up' and draw really concise 2d sketches I get really slow sketches and Fusion does a terrible job of handling constraints. I can't get a well functioning 2d sketch like is required of you in a program like SolidWorks. Then when I go back to make changes the whole thing explodes.

It seems like I can go willy nilly making random stuff and it works, but it's nothing manufacturable. Or I can go step by step and make something manufacturable but it's impossible to make changes.

I don't know what I'm doing wrong and it's extremely frustrating.

I'm at month 4 with Fusion and still feel like I'm making fun shapes and nothing that's real.

[O.Tan]

I hope when they do introduce assembly, it will work like how it's now except that it's linked. Cause I really liked the concept of components and bodies. I don't have to care anymore if I want to make it of a single part or start it as an assembly file. And F360 makes it real easy to move a component into a sub-assembly or even moving it out, feels much more intuitive and don't need to use a special command (transfer command in SE). 

And not sure if some of you guys are aware, but in DM it's possible to move sketches into different components (my personal reasoning to do that is to have an uncluttered sketch panel in the main assembly), but this method also works with Components; moving existing components into another sub-assembly.

https://screencast.autodesk.com/main/details/27ae9e02-3f1b-49ed-a334-5e3e6ad27f17

[daniel_lyall]

I have started to break up drawings to parts that go with other parts, they are done one big picess at a time so the hole thing whont have to be redone if a part goes funny I wont have to redo a big chunk or start again then I can put it togetther and if its all good I delete the bits.

the one I am doing now is a arm to go on my wheel chair so I can sit my lap top in frount of me.

I have done it in 3 bits the arm on the chair what everything goes on (I will keep this bit), the adjustable arm for the laptop table what is a addjustable in every direction, then the table it self.

this is manly jue to one part gets made on a lathe (the adjustable arm), the table I will be cutting on my router

[Anonymous]

As far as I can tell, in DM, sketches have no value after they've been used for a feature of some kind. They are merely reminders of something you did before. They dont link to your body creation operation. You can't edit or re-extrude or anything. You can just delete your body and start again.

Now if DM mode had 3d relationships (your sketch solver solves 3d relationships... dot dot dot 😉 ) and driving PMI style dimensions... hooo boy. 🙂

[O.Tan]

What do you mean by you can't re-extrude? Just turn it back on and extrude from the profile.

It's strength lies in this, let say I have 3 components, A connects to B and B connects to C.

On part B there's 2 holes and its mirrored so a total of 4 holes, 2 holes is for A and another is for C.

Because of how Fusion sketch works in DM, with a single sketch, I'm able to make all the holes (total 8 holes) from a single sketch. And that's very powerful in my opinion.

And driving PMI can already be done in history and that's where history is better at (compared to DM)

[Anonymous]

I mean that in DM if you draw a sketch and extrude, there's no point in really keeping your sketch around. Any modifications to the body after you do more work to it must be done with press pull or move or other similar tools. The sketch isn't connected to anything so that's why it can be moved into any component at any time. This is like how SolidEdge Synchronous works except it doesn't matter because you can drive your 3d geometry with 3d PMI style driven dimensions, 3d constraints, and live rules, and a much better triad (SE: "steering wheel")

I *suspect* that Fusion team decided to use a 3d solver for their 2d sketch geometry so that it would be a quick transition to 3d constraints and dimensions. I also think that no one is really commenting on the PMI thread because this is in the works. If I recall, Fusion started out as a DM tool primarily and then they added History, probably to increase the utility of the product while they really nailed down DM behind the scenes. It wouldn't surprise me one bit if they moved heavily into DM here in the future. Just a theory.

Driving PMI can be done in history but not as concisely as in Synchronous. You can have your dimensions bleed through into 3d space but it's all of your dimensions not key ones. And you also can't show dimensions on things like extrude or revolve features.

[HughesTooling]

Also in DM what's the point in the extrusion showing in the browser when you can't edit it. You'd think you could change the height or select a different sketch. If you add a hole or a fillet you can go back and edit that so why not an extrusion.

Mark

[Anonymous]

This is one of my biggest gripes with DM the way it is now. Lets say you extrude 30mm and you need it to be 40mm. Instead of making some kind of driving dimension, you have to offset the face 10mm.

[jeff_strater]

Hughes Tooling:  I understand the desire, but ufortunately, this is just kind of the nature of Direct Modeling.  Direct modeling is maniuplating the model in its final form, by pushing and pulling the model.   It's not history-based, so in general, you can't go back and edit things.  There's no "rollback".  That's why we added History-based modeling as an option, to give you the choice.

As we developed DM, though, we did realize that, for some operations, we could do a pseudo-edit.  For Fillet, our modeler supports "reblend", which is a local modification of a fillet face, keeping the tangent conditions to adjacent faces.  So, we added an "edit" option to fillet.  All this really does is call Press/Pull on the faces of the fillet (try both and you will see that they are the same).  Similar situation for Hole:   What "edit" on Hole does is just delete the faces of the Hole, then launch you into the Hole command again (it does stash away the settings to make the new hole similar to the old hole).  But, this is kind of the limit of direct modeling.

Extrude is much harder.  Yes, in a simple case like an extruded rectangle, with no geometry added afterward, Fusion could probably do the same trick as for Hole:  delete all the faces and launch you into Extrude again.  But, think about Extrude in general.  You can create a lot of complex geometry with an Extrude, that you cannot just delete and have the model heal back to where it was before the Extrude - it's too easy to consume lots of geometry than cannot be put back together (kind of a Humpty-Dumpty problem).  So, we chose not to try to separate out the simple cases (even detecting these cases is a challenge, I suspect).  By the way, it is possible to get Hole into a similar situation:  Make a big enough hole so that it wipes out something significant, and edit will not return you to the original state.  Or make a "corrupt" hole with later features, and edit will be unavailable.

Now, it is a valid question to ask:  "why put the 'features' in the browser at all?".  And, this was a controvery even within the team.  The "feature" here is mostly just an easy way to select all of the faces that are associated with that feature.  So, if you have a boss or a pocket that you want to color green, you can manually select all the faces and apply an appearance, or you can select the feature in the browser and get the same result.  We have had people ask to just take out the features that you cannot edit, and I understand that request.

Hope that helps clarify the "direct vs. history" topic at least a bit.

Jeff Strater (Fusion development)

[HughesTooling]

I've not really used direct modeling, this thread made me try a few things. If we use the simple box as an example and you need to resize to an exact overall length just to make it a bit more difficult say you start with a length or 50mm but when you come to edit you've forgotten that. Now you want to change it to 52.2mm you can't really drag it because you have no reference for the new overall size. Modifying a sketch dimension would be easy, so is there going to be anything like adding dimensions to a 3d part.

Mark.

[jeff_strater]

No, we don't really have any plans to try to support general 3D driving dimensions.  It would be nice, certainly, but lots of other priorities.

Jeff

[Anonymous]

Hey, what's life without dreaming a litte, right Jeff? 🙂

Hugh that's how Solid Edge "Synchronous" works. You work in a direct modelling environment and apply 3d constraints and 3d driving dimensions. When you're done you have a 3d part that is dimensioned exactly like a 2d draft/sketch  but everything is driven... need that bolt circle to be 125mm BCD instead of 130mm? Just change 130 to 125mm and everything updates including your drawings. You can quickly export it into the 2d draft environment and also as a 3d PMI model like 3d PDF. Even tolerances work and sync between all forms of the part... model, 2d draft, 3d pmi. Those Germans really know how to make some slick tech. Also really expensive tech..!

Fusion is perfectly capable for product design and has a lot of features for designers and hobbyists that SE can't even touch! but as far as the DM environment to beat I give that to SE... there may be others too but SE is the one that has 'captured my heart' so to speak... haha. 🙂 The SE guys told me that when I left it would feel like a tragedy and that's largely true, but as much as I talk up SE it's definitely stuck in the 'old days.' Expensive, esoteric, no integrated CAM, poorly documented, etc. But it's also designed for the mechanical engineering "industry" which as far as I can tell is not what Fusion is aiming for directly. Two pieces of software in the same realm with very different goals...

[kb9ydn]

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@Anonymous wrote:

Didn't even know you could do a DM feature in a history document.

So we have:

DM document, DM components
History document, History components
History document, DM Components & History

Now all we need is DM document with History components & DM components.

Or in other words... assembly document with linked components in other files... like every other CAD program 😉

---

In pondering over this for the last couple days; it occurs to me that when Fusion is finally able to support external file references, it will be mandatory to support DM and history based files at the same time.  If you have a DM assembly and want to add a HB (History Based) component, it would make no sense to require that HB component to be flattened to DM.  Similarly you would not want to suddenly require history collection for a DM component file that gets inserted into a HB assembly.  Fusion will have to be able to switch between DM and HB depending on what item is active in the tree.  It will be very interesting to see how they make all of this work, as I can see some potential mine fields with the infinite number of permutations available.

Interesting times indeed!

C|

[Anonymous]

As I continue to work with Fusion I begin to appreciate more the differences between DM and history. I have found that if you dont think about it and just plow through history mode and make edits via history when possible it works quite well. I think my biggest complaints come with trying to find the right history entry when I want to make a change. There are also few good ways to "clean up" a history bar that is approaching aforementioned "geolocigal scale."

Right now when I put my mouse over an extrude operation, it shows this fairly ambiguous highlighting on certain faces:

Wouldn't it be nice if it showed the actual extrude geometry super-imposed over the existing geometry?

[Anonymous]

Well I'm going to have to focus building my new cnc design for awhile, and wanted to say thanks for this great discussion.  Also wanted to leave you guys with two thoughts, the first 'simple' the second perhaps not so much.  As Luke said, good to just go with the flow in general with the timeline, and if gets very large, I'm guessing areas of it can be fairly easily consolidated.  I would say specifically areas where were working on one or few components for awhile without any work/interaction with other components.  Such a timeline area could be grouped (just like a group that is auto created when insert a Fusion360 part), and would logically represent that component or group of components that were worked on together, in isolation of other components.  The second thought, deals with how I found there actually is a way to quite easily move a sketch when move corresponding component, in such a way that if then edit that sketch, it will not revert back to its original position.  This is particularly useful if make a sketch and component A from it, then decide to move component A to somewhere else, to say interface with component B, and then want to project a feature of component B into sketch for component A, such as in order to drive a feature of component A from the projected feature.  Since component A sketch was not drawn in new position, would normally need to make a new sketch, since the snapshot of new component A position was taken after creation of the sketch, so when edit the sketch the timeline reverts to that earlier time, before position snapshot was taken.  However, so long as the sketch is defined by the moved component A coordinate system (done automatically if sketch made inside active component A, or if not can redefine the sketch to component A coordinate system), then can simply drag the snapshot before the sketch in the timeline.  This snapshot represents the updated component A coordinate system xyz position (and angles), so by placing it before the sketch defined by that coordinate system, the sketch will then have that updated position corresponding to the move of component A, even when editing sketch!  This even works for moving multiple components at once, the moving of their corresponding coordinate systems all being captured in that snapshot.  Note that to move snapshot back in time, ahead of one or more sketches, need to be sure the component creation events (cubes in timeline), corresponding to components that were moved and captured in snapshot, are located before relevant sketches in timeline.  This is because the snapshot of those component moves cannot go earlier than the creation of those components!  If need to, simply move component creation events back far enough in time, which has not caused temporal conflicts for me (unlike moving something forward in time).  Now remember, when make joints, no snapshot is created for when components are moved by the joint tool, so either use move tool in component selection mode instead, and/or my favorite, the align tool, which can align faces, lines, points etc.  Once two components are in proper relation with each other, capture that snapshot to be moved back in time ahead of sketch(s) if needed, and then can use joint tool to rigidly lock components together.  This is all probably almost impossible to understand by reading, and I hope to make a video showing all this in the future.

All the best,

Jesse 

[daniel_lyall]

and they said you cant go back in time

[Anonymous]

🙂

[Anonymous]

Wibbly wobbly timey wimey!

Lol. Every time I use Fusion it feels like an episode of Doctor Who! 

[Anonymous]

Haha, we'll become expert time travelers yet.  I just wanted to add that dragging an event like say a snapshot back in time seems to sometimes be a little laggy, I would guess because the program is trying to figure out if the requested jump back in time is even allowed.  So a little patience helps, just hold the cursor at the desired location between two events until the little indicator jumps there, going back one gap at a time or in larger jumps.  

Good adventures,

Jesse

[Anonymous]

last detail I forgot, is if the sketch that want to project a feature into, is located earlier in the timeline than the sketch or body that need to get projection from, then the sketch/body that want to project from will not be visible when editing sketch.  Can move in time the sketch to edit (and likely all need to also move its related body, such as an extrude) after the sketch/body that want to project from (or vise versa, move the stuff to project from back in time ahead of sketch to edit) so that stuff to project will then be visible when edit the sketch to edit. 

Alright, I'm done for now 🙂

Jesse

[daniel_lyall]

the problems with all this stuff its good for now in a year or two when everything is working better a lot of this stuff is going to be wrong. so much to rember