Still having trouble projecting hole locations from one part to another

[johnAMKDR]

Hello All,

I have received some tips on this but I can't get it to work more than half the time. I have attached an SAT file because F360 doesn't offer f3d because of the linked parts. It doesn't offer f3z for some unknown reason. It's been suggested to break the links, but then I wouldn't be sharing the problematic design. I realize that SAT probably has the same problems.

edit: it seems F360 doesn't make a valid SAT file, or can't tell one if it did:

Correct the highlighted errors and try again.

• The attachment's big assy feb 2 working copy v1.sat content type (application/octet-stream) does not match its file extension and has been removed.

Try a STEP file....

Since Screencast is dead, I recorded a video with Zoom and it is attached as well.

Let me know if these file types are unusable.

John

[TheCADWhisperer]

In the video - I never saw you make the Component active?

[johnAMKDR]

No, I didn't. I'm not sure if I did in other examples when the process worked.

I tried just now. After finishing the sketch, if I hover over the sketch in the browser, purple circles appear on the sketch in the window, but if I click the browser entry, or edit the sketch, they vanish when I bring up the Hole tool.

[jeff_strater]

A couple of comments:

1. by not activating that component, the sketch you create will go into the root component.  I can't quite see, from the video, whether the sketches folder in the root component is visible, but that can be one reason why the projections do not show up.  Also, you want to activate the component anyway, so that the sketch will later move with the component (see point 2).  The other reason why sketches might be hidden is here:
   
   make sure that "sketches" is checked in Object Visibility
2. you refer to the problem of axes or sketches not moving with components.  This will happen if you do not activate the component before creating the axis or sketch.  Activation assures that the component will own new objects like bodies, sketches, and work geometry.  This is important
3. Even if the axes, sketches, etc are owned by the component, you need to understand how Move works with components.  First, make sure that, if you are moving components that the type is set to Components, not Bodies (which is the default).  Second, moving a component just enables the "capture" UI:
   
   You must capture the component position to use it.  But, also, remember:  Capture is a feature in the timeline.  The capture will be in place for things to the right of it in the timeline (new sketches, etc), but if you edit an earlier sketch, that will be before the capture, so it will not be in effect.

Unfortunately, a STEP model is not too helpful here, since it does not contain sketches, work axes, or features.  You should be able to export an F3Z of your design.  That will be more helpful here.

[johnAMKDR]

@jeff_strater thanks for all the tips. I recently got a little coaching and was advised to explicitly activate things. He also suggested that I not use linked components, which I'm not too sure about but I can see that it prevents problems.

Point 1: some of my components cannot be activated. The ones I've noticed have links. Sometimes Fusion will refuse to break the links. I have had some success with edit in place, especially for getting the hole function to find something to cut. At the moment all the objects are visible.

Point 2: in one component, the axes were created when the part was modeled. It's the only body in the component. I edited it, removing the old axes and explicitly activated the component level in the tree and added new axes. When updated in the assembly, the axes move with the component (?, see below)-GREAT!

Point 3: On my system, Move has Components as the default. The part discussed above cannot be selected when Move is set to Bodies.

But honestly, I'm not sure whether this thing is a body or a component. When I find it in the browser, it's icon is 3 stacked cubes, and the link icon. It contains 1 component and that contains 1 body. If I hide it from the browser, it disappears. I can show it by right clicking either the component name or the top level in the browser and selecting "Show all components". However, if I hide it from the window by selecting, right click, Show/Hide; I have to use "Show All Bodies", from the top level. So, is it a body or a component, or some of both, depending?

Point 4: " You should be able to export an F3Z of your design. "  When you say it like that, it should "Just Work", no reservations or special cases. But sometimes it doesn't work for me and there is no option for f3? files.

I will practice with your suggestions. If you can think of a way to get an f3z file created, I will send it to the forum.

[jeff_strater · Accepted solution]

Thanks, @johnAMKDR, 

OK, first one first.  This is admittedly VERY confusing.  But, the reason why you don't see Fusion Archive (F3Z, F3D) in your list of export types, is the method by which you chose export.  You exported the root component from the browser:

That, unfortunately, is a different path than the main export function, from the file dropdown:

Try that method instead.  The "reasoning" around this is, IMO, weak.  But, basically it is:  You can export any component in your design, including local components.  For any component in your design that is, say, a part in an assembly, Fusion Archive does not make sense, so only the standard export types that you see in the list are available.  However, the root component is different.  It does represent the entire design, so, IMO, Fusion Archive should be available from that option, too.  Instead, all components are treated the same, meaning no Fusion Archive, even for the root component.

I'll address your other points in a separate response.

[jeff_strater]

OK, some of the other points/questions in your post:

"I recently got a little coaching and was advised to explicitly activate things. He also suggested that I not use linked components, which I'm not too sure about but I can see that it prevents problems."

I am OK with half of that coaching.  Regarding components, there are two workflows:  internal components, and external (linked) component.  Both are valuable, and have different advantages.  As long as you are aware of those differences, I would not recommend avoiding external components.  Just realize that there are limitations:  You cannot, for example, drill a hole through an external component from the top level (unless you edit in place).

"some of my components cannot be activated. The ones I've noticed have links"

Correct.  That is one of the differences.  What "activation" does in a local component, really, is dictate ownership of new things like sketches and work geometry.  Ownership in external components is dictated by those designs residing in a separate file.  So, activation of an external component would be meaningless.  The equivalent to activation for an external component is either "open", which opens that design in a new tab, or "edit in place", which opens the external design, but in the context of the parent assembly.  Ownership of new object is determined by editing that other document.

"On my system, Move has Components as the default. The part discussed above cannot be selected when Move is set to Bodies."

I think if you have done a Move Components in a session, then, yes, Move will remember the last choice and use that for the next invocation.  But, if you closed Fusion and re-start it, it will default back to Body.  Also, if you are choosing Move from a context menu, it will set the type to the type of the object selected.  So, if you right click on a body, and choose Move, it will be set to Bodies.  If you right click a component, it will be set to Component.  Finally, referring back to the internal vs external component discussion.  You cannot do Move Body on an external component.  Body move is defined to be a document-modifying operation (like adding a new sketch or extrude), so you can only do Body Move if you are editing the external component in a separate tab, or Edit in Place.

"But honestly, I'm not sure whether this thing is a body or a component. When I find it in the browser, it's icon is 3 stacked cubes, and the link icon. It contains 1 component and that contains 1 body. If I hide it from the browser, it disappears."

A couple of things packed in these sentences.  First, it is important to understand Body vs Component, so being able to tell the difference is important.  Fusion does not have a different name for a "part" vs an "assembly".  Both are "components".  If a component has one or more child components, it gets that "stacked cubes" icon, otherwise it gets just a cube icon.  Bodies always have the cylinder icon:

and yes, at both the component and body level, Fusion supports visibility override from the parent component.  So, even for external components, you can turn off a body or the whole component, without editing the referenced design.  This visibility setting is stored in the parent design, so does not affect the referenced design

Hope this helps

[johnAMKDR]

@jeff_strater Thank you very much. Looking back at a search for "why can't i export a f3z" I found a reply from you that advised "file/export". I thought (reasonably, given my experience with many other high-quality applications) that right-click/export would be the same thing. I mean, we have lots of ways to hide a component and they all work the same. Or do they?

This of course highlights a major fault in Fusion 360 in that it is not internally consistent, at least to a new user. A word can have the same meaning, but different uses, or a given word can have two meanings in the same assembly. 

Admittedly, I haven't gone this far in any other CAD program  (Cadkey, SW) but it seems a large part of the learning curve for F360 is learning about the quirks which keep it from working as expected.

I hate my iPhone, but Apple has come pretty far with the "it just works" attitude. Imagine if all of these people weren't cluttering up the forums or watching youtubes and were actually making things. I cannot  honorably bill for time spent on figuring out how to produce an archive file so that I can get help on some other point.

I hope you have some people hard at work to improve the usability and gauging the user intent. And it would be fantastic to click "more info" and actually get more info. How about letting the users enter their own info like for "no body to cut", when the body is obvioiusly there and in the right direction, might mean that it is linked ("read only") and you have to deal with that. 

I'll hold off on uploading the f3z until I've put some time into applying the tips I've picked up recently.

John

[johnAMKDR]

@jeff_strater 

I never got around to uploading the zip file; there were some odd things like a part with slots and the slots were off in the air beside the part. I did eventually get some parts made that so far only have a problem with some countersink diameters. My screws have bigger heads than the default (I know this now). Still, you can't edit the diameter where you would expect to, and the alternative has given almost nothing but error messages. More on that later.

All the tips have been useful, but I would still like to understand the reason for the separate entities of bodies and components. I am gathering info on the different behaviors but not the why. 

Thanks again!

[TrippyLighting]

A component in Fusion 360 is equivalent to a part for example in SolidWorks.

A component is a collection of those objects (in the browser) and features (in the timeline) that help us create the geometry of the component.

A body is a contiguous piece of geometry.

The geometry of a component cane be comprised of one, or more solid or surface bodies. In most mechanical designs each component has only one solid body.

A component also can contain the sketches and construction geometry that were used to create the geometry.

[jeff_strater]

in addition to what @TrippyLighting said, here are a couple of leaning units on bodies/components:

• https://help.autodesk.com/view/fusion360/ENU/courses/AP-BODIES-COMPONENTS-GS 
• https://help.autodesk.com/view/fusion360/ENU/courses/AP-ASSEMBLY-BODIES-VS-COMPONENTS