How to move a component relative to global coordinate system?

[david.antliff]

I've imported an M3 bolt into my design as a new Component. It has a local coordinate system such that the Z axis is parallel to the length of the bolt. However in my design I want the bolt to lie along the X axis.

So I rotated the Component (not the Body) 90 degrees around the Y axis, so it lies along the X axis. So far so good.

However now I want to translate it 8mm in the global Z direction, but when I do this, it moves 8mm back on the global X axis. Turning on the component's origin I can see that when I rotated the Component, its local coordinate system also rotated, which makes perfect sense to me. But what doesn't make sense to me is why a translate of a Component is relative to the Component's local coordinate system and not the global system?

How do you translate a component in the global coordinate system, regardless of its local system?

[TrippyLighting]

The question is why would you want to do that ?

To assemble components the joints in the Assemble menu are the better choice

[david.antliff]

Ok, I haven't really tried assemblies yet - I thought that it made sense to model the M3 bolt as one component, the M3 nut as another, then my two housings (which are to be bolted together with the bolt and captured nut) as two additional components. Can you briefly suggest how I'd transfer this to an Assembly model please?

[davebYYPCU]

Your Fusion file is an assembly file, all in one, 

no changes needed, yes you would have 4 components as you listed them,

some things are built in place, others imported / built on their own origin,

and then jointed.

Might help...

[david.antliff]

Right, so the bit I was missing is that I need to use the Assembly tools to combine the components, rather than simply specifying global coordinates for each? In that case, how do I model clearances? Can Fusion 360 model a nut moving on a thread? I'm intrigued but I don't quite see how it all works yet. I'll look for a tutorial somewhere...

[davebYYPCU]

Right, so the bit I was missing is that I need to use the Assembly tools to combine  assemble the components, rather than simply specifying global coordinates for each?

Correct  (Combine is a tool in the modify menu, and would not be what you mean)

In that case, how do I model clearances?

Dimensions and offsets, with sketches or joints

Can Fusion 360 model a nut moving on a thread?  

Yes, the Nut with a Slider joint - with a motion link to the bolt's Revolve joint.

I'm intrigued but I don't quite see how it all works yet.  

That's understandable, but we try to answer questions - Autodesk has a link at the top  of this Forum for their video tutorials, and a section in there on joints and assemblies.

Might help....

[ToddHarris7556 · Accepted solution]

Sorry, a bit of a long (10:30) video, but just sharing a couple of thoughts on part creation, assembling, and animating. 

As Peter said, there are loads of tutorials out there with more details, but these are specific and pertinent to your question. 

[david.antliff]

Thank you, I will watch this.

[david.antliff]

@ToddHarris7556 thank you again for this. So, if I'm creating my own components, say a simple rectangular beam that slots into a receiver, and I need to model, say, 1mm clearance all around the sides of the slot, then I should "join" based on the centre points of the beam and the slot, such that the clearances are "just there", rather than joining with one surface of the beam (say, the bottom one if gravity is the dominant force) against one surface of the slot? So the beam will "float" slightly within the slot, but honour the clearances I need to have reflected in the full assembly. Is that right or do I need to think about such clearances differently?

[david.antliff]

@ToddHarris7556 sorry, one more related question about your screencast - you mentioned near the start that the components can just float around in space, however when I'm modelling separate components I often need them to be "assembled" so I can model the interfaces correctly. Am I right in thinking that you're essentially saying I should just model each component "somewhere" in global space (doesn't matter where), and use the Assembly tools to bring them together for interface editing, but the individual components always just exist "on their own", floating around in space somewhere? This would be in contrast to what I currently do which is "in-place" component creation, but I'm starting to wonder if this is not the right approach and I should be using Assembly joints as part of my process.

[TrippyLighting]

What @ToddHarris7556 is showing in his screencast is a bottom up technique where you use components you already have either already somewhere else in your assembly, or imported from McMaster Carr or inserted from the data panel.

In many cases, however fasteners for example are used later in the design. One strength of Fusion 360 is top down design. In essence components are designed in their final location in the design. Many (most ?) designs are a mixture of top-down and bottom up design.

To use your example of a beam and and receiver these would be modeled in place, because you don't have existing designs for them and they might only be used in this particular design. You'll also have to assemble them but could use one of the as-built joints in the assemble menu.

Then at some point in time you want to bolt them together. The bolt you insert from McMaster Carr and it will first "show up" at the top level origin of the design. From there you can move it closer to the location you might want to assemble it to. The first move in the insert dialogue is free in the sense that it is not recorded in the design history. So move the part to a convenient location for later assembly.

Then create a "normal" joint between the bolt and the beam.

Clearances im most cases are not modeled but are defined as manufacturing tolerances on the technical drawings for the individual parts. However, for 3D printing for example that does not work.

In such cases I would design to nominal dimensions and when done with the design and at the end of the timeline I would use surface offsets to create these clearances.

And while I am at it, cosmetic fillets and chamfers should always be the features in the timeline.

[ToddHarris7556]

My comments on all of the above were assuming a 'bottom-up' design approach, based on the fact that you said you were importing components. If you start with a bunch of components that are either linked in, or just downloaded right into your model, then you're starting from the details, and working your way up toward a big picture. i.e. 'bottom up'.

Alternatively, if you start with the big picture/layout, and then drill down toward more details/parts along the way, that's 'top-down' design, sometimes called called skeletal or muscular modeling. 

Many projects use some combination of the two, usually skewed one way or another. In this instance, for example, all you really need to know is that the OD of the fastener is 3mm. Draw your layout, with a 3mm placeholder to represent the bolt, and then model away, creating components as you go. Toward the end of that, you'd want to drag in your external components, and place them using joints. 

[davebYYPCU]

Don't make it any harder on yourself, your process is perfectly logical.  

All you need to consider, is that all components are free to move until restrained.  

You have to do something to restrain them.

From Todd's video, the bolt is inserted, bolt Origin to file Origin, he

Click and drags the bolt to anywhere,  it is free to move at this stage of design

you will be given the option to save its new position with Capture Position.  

(Fusion records this position but it is still free to move)

He did not want to save this new position and did not accept the option, it bounced back to its inserted position.

Now you know that, that component needs to be secured, with ground, rigid grouped, or Joint to suit your design.  He uses Joint to accomplish the design intent for that bolt's position.

Now that the bolt is secured, you can model a custom nut component in situ - modelling with the assembled interface - just that it will be free to move, until you restrain it.  

or you can model the custom nut elsewhere and restrain / Assemble it later.  

Fusion has that flexibility, built in, only you know the best option for your design.

Might help....

[david.antliff]

Thanks everyone for your thoughtful and considered responses. I understand the top-down and bottom-up approaches better now, and how a typical workflow would incorporate parts of both. It's all falling into place the more time I spend with the software and on this forum.

Aside: I am indeed designing for 3D printing, so clearances are pretty important. Up until now I have been sizing the components with clearances included, which often results in things floating in mid-air (slightly) but I'll look into surface offsets because it would be nicer to model components to relative exact dimensions and then have a way to adjust the clearances separately, in case I need to change it later.

[david.antliff]

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@TrippyLighting wrote:

And while I am at it, cosmetic fillets and chamfers should always be the features in the timeline.

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Sorry, hopefully not a dumb question, but is this comment related to 3D printing designs or all designs? "Should always" as opposed to...? Is there another way to do fillets (outside of a 2D sketch)?

[ToddHarris7556]

FWIW on the subject of clearances - 

Our workflow is to design these in specifically, as a separate item from tolerances. In our case, a module may consist of several different materials. When we send a prints to our acrylic dept, metals dept, and wood dept, we'd expect that all the parts come back and fit. Since all the materials have different thermal coefficients and hygroscopic properties, we use clearances to assure that the parts won't self-destruct when the temperature or humidity change 🙂

There are lots of ways to approach that - offset planes, sketch parameters, etc. It's as much (or more?) about understanding your materials and design needs as it is understanding the software.  

[david.antliff]

@ToddHarris7556 that sounds reasonable. In my case the 3D printer I use isn't 100% dimensionally accurate - it has a small fixed error (and an even smaller proportional one), due to spreading of the plastic as it extrudes. For example, a 5mm wide beam will print at, say, 5.10 wide, and a 5mm slot will print at, say, 4.95mm. I've worked out that a clearance of 0.15mm per face gives consistent and acceptable results, so in order for them to fit properly I need to design the beam for, say, 5.00mm, and the slot at 5.00 + 2 * 0.15 (two faces) = 5.30mm. I don't need to reduce the beam dimension, but I do need to retract the slot faces slightly (I could do a mix of both). But if I just print them at nominal 5mm then they simply don't fit together at all.

[ToddHarris7556]

Not a dumb question at all. Two quick thoughts based on my experience:

1) From a geometry perspective, fillets and chamfers tend to be pretty low on the priority chain. Put your major modeling features in first, then add fillets later. It makes for a more robust model. If you try to add major features after fillets have been added, you're much more likely to run into modeling challenges. It'll sound like a dumb analogy, but I can't think of a better one : make sure the cake is the right shape before you put the icing on it. Once the icing is done, changing the shape of the cake becomes a whole lot less fun.  

2) I would say the vast majority of chamfers and fillets are non-mechanical in nature.  i.e. they're there for deburring, safety, mold release, etc. A valve seat, or other mating surface, would be an exception, but I would suggest most are really non-critical. 

In any event, if you stick them in at the end, it's easy to roll back the timeline and just shut them off. If you need to alter underlying geometry, this will save lots of headaches. Once your edits are done, turn them back on. 

Re: 'other ways' I don't know that there's an absolute rule on this, but in some cases, it might be easier to sketch underlying geometry square, and add the fillets as 3d features after. There's certainly more control over your fillet application, and it offers the benefit described above (being able to turn them on and off as desired). Personally, I know that I sketch some in, and I add some after. It's probably better practice to add them all in after. 

[TrippyLighting]

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@david.antliff wrote:

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@TrippyLighting wrote:

And while I am at it, cosmetic fillets and chamfers should always be the features in the timeline.

---

Sorry, hopefully not a dumb question, but is this comment related to 3D printing designs or all designs? "Should always" as opposed to...? Is there another way to do fillets (outside of a 2D sketch)?

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As a general rule I try to keep sketches as simple as possible and anything that can be modeled using a modeling feature will be kept out of the sketch. That generally applies to fillets and chamfers, pattern and mirror operations.

Sometimes it cannot be avoided putting a fillet or other detail into a sketch but simpler sketches are more stable and are not as easy to break as complex ones. 

This applies to all parametric CAD software, but particularly to Fusion 360 sketches. The Fusion 360 sketch engine is a new development and as such suffers from performance problems and bugs. 

In parametric CAD software existing geometry is very often used as reference for new geometry. As such it is best to keep cosmetic features or features that are not essential to the function of a design at the end of the timeline to keep these references earlier in the timeline "healthy".

[david.antliff]

@ToddHarris7556 @TrippyLighting thank you both for your replies. That makes perfect sense to me. I've also discovered that keeping sketches simple and using features for mirroring/cloning/filleting/etc helps significantly with performance. In an earlier design I tried to add all of my eventual profiles to a single sketch and the software ran very slowly as a result, so I'm following the "one sketch per feature" rule now and the user interface seems much more responsive as a result.