Modeling Exclusion Areas

[bloudraak]

Assume for a minute that I have a design of a panel that accepts panel fasteners.  Some things, like PCBs, are mounted to that panel. 

The panel fastener has a diameter of 10 mm but requires a clearance of 7 mm from the center to any edge. From a practical perspective, that clearance should be more like 8mm or 9mm, so a human can use their fingers to tighten or loosen the fastener.

I've been using a circle on a sketch for the clearance. Which requires me to visually inspect clearances. 

So how would one model such a clearance so that I can use Fusion 360 tools to report interference and whatnot? It's almost like having an invisible body around the fastener. 

[hamid.sh.]

I think you yourself have answered your own question; make components representing each clearance, make them low opacity or totally invisible, joint them with fasteners. For simple selecting or hide/show nest them all in a single "Clearances" component. Also you can make them Unselectable within viewport (right click) so they don't bother you while modeling. When checking for interference select this "Clearances" component from the browser.

[bloudraak]

Thanks, @hamid.sh., I had a go at creating a clearance component but got stuck rather quickly. 

In this case, I'm trying to model clearance for a PCB device. It's the same principle as the fastener, just a bit simpler since the device is rectangular. Say I have the following user parameters:

• DeviceWidth: 50 mm
• DeviceDepth: 80 mm
• DeviceClearanceLeft: 20 mm
• DeviceClearanceRight: 5 mm
• DeviceClearanceBack: 30 mm
• DeviceClearanceFront: 5 mm
• DeviceClearanceBottom: 5 mm
• DeviceClearanceTop: 10 mm
• DeviceThickness: 2mm

I'm able to create a sketch for a "Device" of "DeviceWidth x DeviceDepth" and extrude it to "DeviceThickness".  This is the body that I'll use to create holes for where standoffs and corresponding screws need to go in the assembly. 

Now I'm trying to create a clearance component for that device.  Since this clearance is in all directions, I'm assuming the origin for the clearance sketch needs to start at (-1*DeviceClearanceLeft, -1*DeviceClearanceFront, -1*DeviceClearanceBottom) in relation to the Device sketch.  How does one set the origin for a new sketch, and can that be through user parameters?  I can easily infer the X, Y dimensions of the clearance rectangle, which would be something like (DeviceClearanceLeft+DeviceWidth+DeviceClearanceRight) and (DeviceClearanceFront+DeviceDepth+DeviceClearanceBack). But it's unclear how to do so accounting for clearances above and below the device when extruding the clearance body such that Fusion 360 will not report interference between the "device" body and the "clearance body".  

As for clearances in general, I don't see an easy way to model clearances where the standoff or fastener requires a hole that is at least a specific distance from any edge (including other holes, bends, and whatnot). This is one of the areas where mistakes are often made, requiring rework in the design. I was hoping Fusion 360 would help in that regard. 

[TrippyLighting]

I suggest you share a design so we have something a little more concrete to talk about.

[bloudraak]

Attached is an example of a design that represents a device (a PCB or small board computer like a Raspberry Pi, OmegaS Pro) in terms of dimensions, mounting locations, and thickness. The dimensions and thickness are defined as user parameters. Also in user parameters are clearances for the device, which is necessary for airflow, attaching cables, and whatnot.

This design is derived from a template since I have around 45+ "devices", which all occupy a cuboid in space, with standoffs connecting a device to other surfaces, such as a panel mentioned in my original message.  I add the design to an assembly that includes standoffs, fasteners, and whatnot, each with its own requirements around clearances.  In the end, I'd like to get Fusion 360 to identify where there is going to be interference between the various components, or areas where clearances are not met. 

[TrippyLighting · Accepted solution]

I think what you are asking is not just a modeling , but lets start there.

IN order to define the keep-out volume around the part, you can simply copy-paste the body (make sue the component is activated). Then you can push-pull the faces of that copied body by the clearance dimensions you defined as user parameters.

[bloudraak]

Thanks, @TrippyLighting. It never crossed my mind to do that.

When I do check for interference, Fusion 360 reports interference between those two bodies. Is there a way to avoid that? 

[hamid.sh. · Accepted solution]

When I initially read your post I imagined you want a clearance around fasteners only but since you need it in all directions what @TrippyLighting suggested works well for you.

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@bloudraak wrote:

Thanks, @TrippyLighting. It never crossed my mind to do that.

When I do check for interference, Fusion 360 reports interference between those two bodies. Is there a way to avoid that? 

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You can use Combine to cut the original body out of the clearance volume while keeping the tool (so you won't loose the original body):

[bloudraak]

Thanks, @hamid.sh.! That worked great.  

Yeah, the exclusion area around the fasteners is something I'll focus on next.