Fusion 360 help please.

[ajlelectronics]

Doing it's job with temporary software...

 

[My Old Landy]

Doing it's job with temporary software...

View attachment 456554

That does look good it really is worth the effort in the end.

 

[ajlelectronics]

Stuck again and would appreciate some advice please...

The new part (in gold) is a carrier for a module PCB. It is in two parts as well as a combined component for test printing. The front panel with the D cutout is not required, what I do need is to transfer the hole pattern into the rear panel but it tells me that I cannot copy into the same sketch. The module case can probably become part of the chassis rather than a bolt in item, so no fixings are required.

So my questions are, how to get the rear panel cutout and linked to the module case's lateral position?

The D type component I tried to use as a cutting tool, but whatever I did, the component became embedded?

 

[ajlelectronics]

This is a mockup of it.

 

[ajlelectronics]

I have just noticed another couple of 'warning' but haven't had chance to look at them.

 

[Misterg]

So my questions are, how to get the rear panel cutout and linked to the module case's lateral position?

I would:

Create a new sketch on the rear panel;

Project the shape of the module cut-out into the sketch (I've selected it from the menu with the mouse in the video below, but you can just press 'P' when the sketch is open).

Use the sketch to extrude the holes through the rear panel.

Like this:

Normally, I would make sure that I have the component I'm working on selected in the tree on the left (the dot next to it), but your design has got quite contorted (which I think is par for the course when you're learning as you go), and I didn't bother trying to fathom it out!

The D type component I tried to use as a cutting tool, but whatever I did, the component became embedded?

Anything you use for the design is part of the design and F360 needs access to it. You can right click on components and 'Remove' them if you want to reference some feature, but you really don't want them in the finished design, but I'm dubious as to whether that's the right way of doing things here.

 

[ajlelectronics]

I am indebted to you.

 

[ajlelectronics]

Could you elucidate on the D plug please? I thought that I could use it as a "punch" but I could only merge it with the panel, rather than cut it away using the shell of the D plug which I though that I could do.

 

[Misterg]

Could you elucidate on the D plug please? I thought that I could use it as a "punch" but I could only merge it with the panel, rather than cut it away using the shell of the D plug which I though that I could do.

You can use the D plug to cut a hole, but bear in mind that the D Plug component is made up of 18 different bodies, and it is the bodies that will form the cutting tools, rather than the component. There is no one body that represents the panel cutout that I think you're looking for.

You can overlap it with the panel and use the 'Combine' tool with the 'Cut' option selected to make a hole in the panel using the outer part of the plug ('Cut' is the middle selection on the 'Operation' line). You end up splitting the rear panel into two bodies with a narrow slot in between:

If you make the D connector invisible again, you can see the effect (Body69 has been created):

You could then hide or delete the body forming the middle of the hole, but it's a very long winded way to go about things, and probably not the right way to go here (IMHO).

My point above was that if you did go this route, the D plug component still needs to be in the design - I thought that this is what you meant by 'embedded' (an "Embedded component" is something you can add to models) but now wonder if you just meant that the plug became part of the panel?

Next Big Thing: If you want to position components relative to each other DO NOT use the 'Move' command - Use 'Joints' instead (bit of a learning curve, unfortunately!) Or at least make sure to select 'Capture Position' after the move.

 

[Erie Fred]

I build the base model (an .ipt file in inventor) then bring it in an assembly file (.iam file).
add the parts that bolt up to the base model, mate them with dimensions.

Then, while in the main assembly, edit the base model file (the assembly tree will grey out everything other
than the base part).

As above, start a new sketch, xfer the details you want from the bolted parts onto this sketch.

Keep your head about you, to just exactly where your working (the base model, not the assembly).

 

[Misterg]

Keep your head about you, to just exactly where your working (the base model, not the assembly).

Fully agree. Unfortunately(?), by default, F360 puts the operator straight into the assembly when you start a model (without making it obvious that this is what's happening). It lets them start creating things without any need to think about bodies, components and assemblies and the way that the model will fit together - for example it lets you create bodies that are part of the assembly, rather than a component. This sort of works for simple parts, but doesn't teach them how to work, and falls down rapidly once things start getting more complicated.

*THE* best thing to do when starting a F360 design as a learner is to create the main components before you do *any* design work - e.g. 'Front Panel' , 'Rear Panel', 'Chassis', 'Stand-off', 'Module' , etc. etc. then select one of these and start your design. (You can always switch between components and add more components whenever you want to.) - At the very least, create one component and work on that, rather than the default of working in the top level (which is an assembly, as above).

The relationship between components within the assembly is set using 'Joints' - these can be simple dimensions, mating faces, aligning holes, etc.

However, one step at a time...

 

[ajlelectronics]

Another query please...

I want to cut out a 'speaker grille which will be 55mm in diameter. I can use any shape of hole. The circular pattern tool looks interesting and I have played with it a bit, but what would be the suggested way to do it quickly and efficiently please?

 

[daedalusminos]

I would probably use a spiral and pattern the holes along that.

 

[daedalusminos]

I would probably use a spiral and pattern the holes along that.

Like this - you can see the spiral path that generated the pattern...

 

[ajlelectronics]

That all makes sense. Thank you.

 

[bricol]

The more industrial systems I've used allow you to pattern a hole in a circular or rectangular pattern within a boundary, allowing you to set the clearance to the boundary so all holes remain entirely within it, leaving gaps as needed close to the boundary.

 

[Anguz]

how do you draw a spiral in 360 ?

 

[daedalusminos]

how do you draw a spiral in 360 ?

Use the coil tool - in will create a solid helix/coil using the options

 

[Anguz]

Use the coil tool - in will create a solid helix/coil using the options

easy when you know how

 

[ajlelectronics]

easy when you know how

Well I wish that I did! I can create a coil no problem, but a flat spiral is a different matter!