building a box for my vacuum cleaner. (Down another rabbit hole)

[mark33.in.oz]

Sorry folks, this is a real big trip up for me.

This is a bit of a long post.

Only to explain the story - though somewhat academic at this point in time.

But I feel I need to explain how I got here and why to (maybe) help in the bigger picture.

INTRODUCTION:

I have been using Fusion 360 for a few years now but it is only on a limited use and it was done more for 3D printing than where I am now.

Not to detract from what the program can do and I accept its limits.

But recent events have presented me with a whole new rabbit hole down which I am traveling now.

So for the record:

I only "designed" this to get an idea of what I wanted to do and look at how it was going to be built.

Then the situation presented itself that completely changes the course.

I bought a new vacuum cleaner (portable) and want to build it a "house".

I sat down and "built" models on the parts and then the "house" into which it would be put.
This way I could look at item interaction (or how it would look when built) and make sure things were ok.

See the model.

Knowing my luck all the pieces will be everywhere and not where I want.   Haven't worked that problem out either.

Now a "walk through" of the idea:

It is a top/sides and bottom of a box with TWO backs.   1 is the REAL back and the other (in this case) is called the "insert".

Why?

Well, this was done for my benefit for the positioning of the "charger".

At the start I wasn't sure how that was going to attach to the rear wall.   Bolts, nails or.....????

Ends up being two dowels.   There will be washers to fill in a bit of space to fill in the small gap to make it all "level" then a piece of wood (thin) put between the two dowels.

And there is a hole for the power cable to pass through.

That hole also needs to be in the back plane but the two holes for the dowel don't.

So the power cable hole needs to be lined up on both pieces.

This is easy but then lining up the "charger" with the holes is difficult so I hide the "housing" and line up the holes with the "charger" and the holes in the "insert".

Then un-hide the "housing" and move it into position and work from there.

(Sorry, I hope you are still reading this as I still haven't got to the problem yet.)

So with all pieces in place I could see what I needed to build the "house".

This was done by making a drawing of the "house" and showing all / most of the dimensions.

That was kind of painful on my version as I couldn't do all I wanted.

Not sure that is because of the limits of the version or my knowledge.   But anyway.

ALTERNATIVE IDEA:

I showed this to someone for a second opinion and......

Then someone said it could be laser cut easily.

All you need is to export the ...  file in the required format.
(Which ok:  This version doesn't allow)

But that isn't the problem.

I have access to a full version (limited use of for time) and went there with the idea of making/exporting this file.

I "hide" all the non-house parts and export to the file.

Alas ALL the pieces/parts are exported.

What kind of throws the proverbial spanner in the works for me.

QUESTION:

Main one:

What do I need to do?

Delete the non-required parts and then export?

Another while here:

So, the original idea is I make a "model" of all the things and make sure they can "play with each other nicely" in the house I want to make.

But any time I go in and edit a piece/part:  all/most other parts get moved elsewhere/back to their start positions.

Ok, I kind of get that.

But isn't FUSION supposed to be ...... parametric?

And as I am making ... components (separate parts) rather than as I originally did - in one big homogeneous mess - shouldn't they remember where I put them?

I know this is a big ask and it will be difficult to help me.

I am not even sure I am going to be able to understand what will be said/told to me via the group as "SIMPLEX" "HALF DUPLEX"  (two way communication with long delay between who's talking)  communications are not easily processed by me.

I'll stop here as I think I have (probably) gone on long enough now and already lost people.

Going on more will only lose more.

Thanks in advance.

[TheCADWhisperer]

@mark33.in.oz 

I decided that two Mirror could be replaced by one Circular Pattern feature.

Make Sketch1 visible again.

Go to Extrude and set to Thin Feature.

Turn off Chaining selection and then select one edge as shown...

Go to the Combine tool.

Set the side body as the Target Body and the back as the Tool Body.

Set to Cut and Keep the toolbody.

Mirror the body to the other side...

Thin Feature Extrude the top.

Combine - Cut.

Mirror the top to the bottom.

Hmmm, we should have added the Finger Joints to the sides before Mirror.  No problem - Fusion is a history-based modeler, we can go back in history. 

Attach your file here for next set of steps. (The next few steps are fun - and very powerful.) (Note that we have not created any complicated sketches. Note that we have not created any additional sketches.  Any sketches that we do create will be created on the Origin Workplanes, not on part faces. (The BORN Technique.)

Any sketches we do create will be fully defined - no blue lines or white dots.

[mark33.in.oz]

> Make Sketch1 visible again.

> Go to Extrude and set to Thin Feature.

> Turn off Chaining selection

> and then select one edge as shown...

Check.

Check

Check

FAIL.

Why did you concatenate "Turn off Chaining selection" AND "and then select one edge as shown"?

When I do that it just fails compared to your screen shot.

PLEASE ONE instruction per line if you want to keep things easy.

I see no advantage in what was gained by combining those two things into one line.

Only to highlight the problem I set a value.

 

ONE SIDE.....   Not happening when I try.

TRAIN WRECK at this end.

[TheCADWhisperer]

@mark33.in.oz 

I used the wrong terminology for Fusion.

I should have said select Line (not edge).  (Sketches have lines, bodies have edges.)

The inclusion of images and a bit of logic should help where the words become confusing.

Select the vertical line from the first Rectangle that we created in Sketch 1.

To see why we Turned off Chaining Selection and selected the Line in one sentence - try it without turning off Chaining Selection.  Experiment and observe.

BTW - I see a lot of stuff after your history marker in your screenshot image - delete all that stuff or start over from the beginning.

[mark33.in.oz]

I feel this is being done to test my patients.

Doing what I understand you are saying - which seems to change with each post - I get another train wreck.

And I shall state here:  I pretty well failed English when I was at school.   So yes it is probably MY FAULT.  (As is everything that happens in the world.)

As you showed me in the picture from your screen shot.

 

 

That is after I click on "one of the lines".

The entire perimeter gets selected, and so the lot gets extruded.  Not as you show it.

To me this means I am not being told what I really need to  do, rather some vague "something like this" which is both wasting my and your time.

I want (am asking for) help that will tell me EXACTLY what I need to do so I can do it.

"All the other stuff" in/on the time line is/are the hooks and wedge who's sketches I need.

I've extruded them so when all this is complete I can make the required sketches so I can then get the needed .DXF files.

Are they hurting what is happening now/here?

I have posted the project and you should be able to see them.

Yes, I did make a mistake with two of the "hooks" being the same size.

That is fixed.  But the question remains:  Does it effect what is happening here and will it at the end when all done?

[TheCADWhisperer]

@mark33.in.oz 

Did you turn off Chain select BEFORE selecting the line or after attempting to select the line?

---

@TheCADWhisperer wrote:

Make Sketch1 visible again.

Go to Extrude and set to Thin Feature.

Turn off Chaining selection and then select one edge sketch line as shown...

---

Your going to love the next set of steps.

[mark33.in.oz]

So to keep things "structured" wouldn't it be nicer/clearer to all if it was more like:

Do step 1

Do step 2

Do step 3

Rather than

Do step 1

Do step 3 but after you have done step 2.

(or)

Do step 2 then step 3

As I mentioned before:   Concatenating things instructions doesn't always work.

Make sketch 1 visible

Go to the extrude feature

Turn off CHAINING

Select one edge of the sketch line

Trying it now.

Ok, that's working.

Now next "derailment".

>  Go to the Combine tool.

Where is this hiding?

I see "Create", "Modify", "Assemble", "Construct" and so on.

COMBINE....   Lost me.

I've checked those menus and can't find a COMBINE in them.

(but may need glasses)

FOND IT!

Hang on.

Ok, moved forward a bit.

Another derailment.

Shown from the back to (I hope) show I've got the two side panels working with their joints.

But when I do the top one.....   I lose the finger joints on the back panel.

This MAY be a better view.  Before i set the thickness of the top piece.

 

After a bit of re-re-re-reading...

This is what I have:

Green = good.

Red:  not so.

Lack of finger joints.

 

EXTREME lack of commands in that.

I had to "thin extrude" to NEW BODY (NOT CUT as you said)

Then do a COMBINE bit with the KEEP TOOL BODY.

THEN I got this.

But to me the finger joints on the original side panel should be made before (a) mirroring it and (b) making the top.

Dunno though.

23:00 local here.

I'm off to bed.

(Until tomorrow.)

Thanks.

[TheCADWhisperer]

---

@mark33.in.oz wrote:

That is after I click on "one of the lines".

The entire perimeter gets selected, and so the lot gets extruded.  Not as you show it.

---

Hmmm, I wonder if I look up the definition of "Chaining" if it might describe the behavior that you observe?

Observation and Logic are important to design work.

Post your file here when you get the sides completed (as per my instructions - we are going to learn efficient modeling techniques - that was my stated goal at the beginning).

[mark33.in.oz]

This is the latest I have got - with a bit of my TRYING to get my head around things and doing more stuff.

I have had less than a good night's sleep since my last post.

I am going out soon to a busy-ish day, and checked for updates and so am replying.

> Hmmm, I wonder if I look up the definition of "Chaining" if it might describe the behavior that you observe?

Observation and Logic are important to design work.

Why are you arcing back to a post that is now resolved?

You told me where i went wrong, I posted that I got that part working.

(Well: I am sure I did)

Yes, in post 68.  I showed you what I got.

So that is resolved - to the best of my knowledge.

Or is it I am still doing something wrong?

Your screen shot doesn't show the top part and so avoids the missing finger joint problem of which I asked.

Yes:  I did "get ahead of you" - sort of, but your instructions were:

(Quote)

Thin Feature Extrude the top.

Combine - Cut.

Mirror the top to the bottom.

So I am not really ahead of you.

[TheCADWhisperer]

I have to make a video for the next few steps as I suspect words and screenshots alone will not adequately convey the steps.  Check back.

[mark33.in.oz]

Only to try and learn these new tricks I've done a bit more.

I think I've messed some of the bits up.   But "not the end of the world" stuff.

The things I've done are more on the hooks and wedges.

Here's my latest effort.

I've also changed a bit of the mechanics of how the hooks and wedges (and back board) connect.

[TheCADWhisperer · Accepted solution]

Check when finished compiling.

https://youtu.be/DNDBcrCfvrQ

@mark33.in.oz 

Can you ask your laser operator about laser diameter for the purpose of adding "dog-bone" joints for ease of assembly.

[mark33.in.oz]

Wow!

That is great.

Thanks very much for that.

Yes, that is a great way of doing things.

I appreciate why you use only the origin axis and that is a good example of how to do just that.

As I am still on my "training wheels" I didn't think of doing it that way.

I'll apply that to my model ASAP.

On a side note:  I exported my effort to a DXF and took it to be looked at.

All pretty good - as mentioned.

WRT the "dog bone" parts:

Ok, but (just mentioning)  I loaded the "original" (new) effort in to their laser cutter program and the finger joints were checked and all was good.

The problem with the corners wasn't mentioned - yes, maybe my responsibility to ask - but the people who have the laser cutter often make boxes with finger joints and they don't seem to need to do them.

Maybe the program does that in the background for them.

But it is nice to see what you mean.

The trick with making the `+` sign then making that into the hole is fantastic.

I would never have thought of doing that.   But I don't have a design background.

I'm still watching the video (while typing this reply) and so the responses are "in time with" the time line of the video.

And 20 seconds further down the video you mention the utilities that may do it automatically.   🙂

Oh, ok.   You were talking in Fusion.   I'll ask them.

But I've seen them design a box, put the wood down, cut it, take the wood pieces out and put it together there and then.

I know there is a setting to adjust how "tight" the finger joints are.   But I'm not sure if that is when they are making the box all from one job, rather than how I am doing it now.

I guess some of my confusing is that I don't fully understand what PARAMETRIC means - and how it works.

When I made my "hooks" and "wedges" I used the edge of their respective holes are the source plane/s.

So that may not be a good thing.

I'll stop here and now to get what you showed me done.

Again:   Thanks.

[mark33.in.oz]

Not a big deal, but you didn't explain "circular pattern" to me.

I think I can work it out.

But is it "circular" or more: "rectangle"?

Just checking.

[mark33.in.oz]

Just touching base with things.

(aka My questions)

1 - the second sketch 4:18.   Ok, the "origin" is at/on the back of the back part.

You make a construction line from there "out" (forward) the thickness of the wood.   Then a second one form the front of that line.    The distance is set to the depth.....

From there you put a vertical line at that line's mid-point.

Problem (for me)

That means the vertical line will NOT be in the middle of the side piece.   It will be offset by "thickness"

I know it is nothing in the greater scheme.   We are only making finger joints.

2 - The "52" is depth / 5 and I picked that just for a nominal number/size of fingers.

(Ok, only 2 questions).

[mark33.in.oz]

Oh, and - sorry.....

So how do I then "project" the bodies to an area where I can then get the DXF file to give to the laser cutter in such a way that if I modify any body, the DXF file reflects the change?

[TheCADWhisperer]

7mm is pretty thin and if the wood is soft it will compress, but just the same, check with your laser guy about the corner reliefs (dog-bone).

I will have to make another video about laying out the Components and Save As dxf of the sketch.

[davebYYPCU]

I may be wrong, but the kerf (mine is 0.2mm) of the Laser is sufficient to account for the (dogbone) corner,

but they would be needed for a router.

@mark33.in.oz  Did you investigate DXFer?

Selects the face of each part, puts them into one file.

While I am here, the last set of fingers will be in the middle of the visible inside face.

Might help....

[mark33.in.oz]

Sorry lost me with "in the middle of the visible inside face."

(And: last set of fingers)

[mark33.in.oz]

Yes, 7mm is "thin", but I'm not hanging the Titanic from it. (as is my seemingly new/recent catch phrase.)

The pieces are less than 1KG weight (each).

The heaviest thing is the vac' and its charger.

But the 2 x 8mm dowel do seem strong enough.

But thanks.

[davebYYPCU]

Tabs / sockets - interlocking fingers.

Side wall inside visible face -

can't see into or past the floor, so 7mm less than the outside face when assembled, 

Might help....