Refurbishing my Voron 2.4 300

[claudermilk]

Awesome tutorial there! Also a very nicely designed case for the screen--the button paddles are a nice clean, elegant solution. It's almost like you've done this before. 

[Penatr8tor]

14 minutes ago, claudermilk said:

It's almost like you've done this before. 

Yes... Appearances can be deceiving. 

Hey thanks for the kudo's @claudermilk 

It's not a super thorough tutorial but, I think I achieved my goal of outlining the philosophy of how and where you start and who knows... maybe it sparks a flame in someone that's been on the fence.

I have one more redesign of this to make it worth posting as a downloadable mod.

The paddle switches work but they feel a little mushy. I need to give them a little more room to move. Also, I need to give the ribbon cable a little more room to loop around under the display. I'll make a little addendum tutorial on how to tweak or modify your design. I think that might help some people.

[claudermilk]

It almost never is quite right on the first iteration. If you get it in two you're well ahead of my simple attempts at CAD; I'm just doing game organizers, which is my original excuse for getting into 3d printing.

[Penatr8tor]

Funny... I have found the term, third times a charm, to be pretty accurate. Even at work we anticipate at least 2-3 iterations to get a design good enough to move forward.

I also discovered that there's already a million really good, clever ideas hiding in existing plastic parts. Long ago, I worked for Racal-Datacom, I designed modem enclosures. My boss had a cabinet filled with random plastic and sheet metal parts in his office. He opened it up and said... Pete... This is the cabinet of ideas. If you need one, just open it up and find one. It'll be attached to one of these parts.    

[Penatr8tor]

As I mentioned to @claudermilk, the display enclosure needs to be adjusted a bit. The little buttons work but feel a bit mushy and they operate correctly about 90% of the time. Over time this will be an annoyance that nobody would want to endure so let's fix it.

As it stands currently, we have just barely enough room between the paddle and the display for the paddle to move back and forth and transmitting a tactile click from the switch. I also need to open up a pathway to route the ribbon cable thru.

So, with all that said and without further ado... Let's get right into today's vid... I mean tutorial. Sorry in advance for the Modbot intro. 

Let's take a look at the switch issue first. Below is a section view of the display, base plate and switch paddle. If you look at the gap between the display (yellow) and the paddle (blue) there's only about 1mm of space for the paddle to move and actuate the switch. The paddle is also very thin. I did this on purpose as my initial thought was to allow the paddle flex back and forth to actuate the switch. Well... it's a little too flexy and the paddle hits the side of the display before the switch is depressed. Also, the pocket that the paddle fits into is really close to the edge of the base plate, literally 0.5mm and only the width of one perimeter when printed.

So, the strategy for this is to.

1. Thicken the paddle.

2. Move the paddle away from the side of the display ~2mm.

3. Increase the base plate size.

One thing I did initially was to create a cross section so that I could monitor what's happening. To make a cross section, I first create a reference plane. Planes are infinite flat planes without thickness that you can use as a part of a framework or scaffold to build things off of, to or from. Since I want to section thru the middle of the paddle, I'll choose the mid-plane command from the "CONSTRUCT" menu. Mid-plane needs you to select 2 flat surfaces on your geometry and will split the difference between them. In my case I'll select the two vertical sides of the 1st paddle (others are copies). The plane is a yellowish-brown color, and it scales to the size of your selections. You can pull on one of the 4 corners to adjust the size without disturbing its position at any time.

To make a section, pick "Section Analysis" from the "INSPECT" menu, select the mid-plane we just made and click OK. Viola! Cross section. On the left side of the screen is the "Browser", near the top is the "Analysis" section (it's kind of like a folder) and you can toggle the section on and off by clicking the little eyeball. This visibility toggle works for everything in Fusion.

OK, let's do our first change and see what blows up!

Because...

 Pro Tip: things will blow up so don't be surprised... expect it and when it doesn't... you will have a good surprise instead of the other kind of surprise.

One of the things people find most annoying when learning CAD is where to find things. For instance... how do you make the base plate bigger? Where do I look? What do I change? This is where a little knowledge of the "timeline" and how it works is valuable. Below is the timeline and it runs along the bottom. From left to right are all the features I created in the order that I created them. If you hover your mouse over one of the icons it will pop up a little info bubble with the name and type of feature and if you hover over a sketch icon it will also highlight the sketch. This is how we find what we want to edit. I've also attached the Fusion 360 file of this enclosure (pre-edit) so that you can open it up in Fusion and edit along with this little mini-tutorial. Enclosure Mello Fly-Screen 7in v16.f3z

For now I have the bezel part turned off (eyeball toggle) so I can work on the base plate. I hover my mouse over the timeline and find that to make the base plate larger, I need to edit the first sketch in the timeline. Just right click on it and select "edit sketch". This is how everything in Fusion gets edited.

If you look at my sketch, you'll see that I drew a rectangle around the perimeter and dimensioned the edges to be 3mm away from the display. I also linked the top, left and bottom dimensions to the right side dimension. This is really easy to do, when you create the dimension, instead of typing in a value... just click on an existing dimension and hit enter. They are now linked. So, If I want the perimeter to be 4 or 5mm, I just change the one dimension and all the linked ones update. Unfortunately this isn't going to work for me because I only want to increase the edge where the buttons are. No worries. We just edit the dimension value (it's d21 currently) and put whatever number we want. This breaks the link and applies the new value.  Pro Tip: d21 is the internal dimension name or designator. For example, if I want the dimension value to be half of what d21 is.. I can click the dimension I want halved and then type "/2" after the "d21", "d21/2" So, if d21 = 3 the dimension would display fx: 1.500, the "fx:" tells you there's a formula.

So, lets change it already. Now you can see that I have a 5mm offset on the switch edge. Let's "Finish" the sketch and see what happens...

OK, no blow-ups. The base plate is 2mm larger and the paddles have moved an additional 2mm further away from the screen. You'll also notice that the 4 pockets that hold the paddles have also moved and that the nub that contacts the switch is now 2mm larger as well. This is because I created intentional dependencies that drive other components.

Let's now move the pockets 1mm away from the edge.

First, we hover over the timeline and find the sketch that drives or defines the pockets or... we can right click on one of the surfaces of one of the pockets and select edit sketch from the pop-up menu. Either way will get you there.

Let's take a look at this sketch. I have 4 center point slots (only 2 shown) along the top edge. Each slot is centered with each switch. To do this I used the "project" command and selected the edge of each switch. Those edges are depicted as purple lines with little circles on the end points. This lets me draw a line from the middle of the projected switch line to the center of the slot. Once I have my first slot constrained. I just use colinear and equal constraints to align and make all the slots are the same size.

OK, let's change the number already. I increased the distance from the edge from 0.5mm to 1mm and also increased the slot height to 2.5mm. Remember, we're making two changes, 1, creating more space between the slot and the edge and also increasing the thickness of the paddle so we need a bigger slot as the paddle thickness is driven by the slot.

 

OK, let's finish the sketch and see what happens... Success and once again, no blow-ups. Of course, we still don't know what affect these changes have had on the bezel. You can also see that not only did the slot update... So did the thickness of the paddle. Those deliberate dependencies are paying off in spades right now.

Well... would you look at that... Looks like the bezel updated without issue as well. Good models make editing way easier.

Let's do a little investigating to ensure that what appears to be correct on the outside is also correct on the inside. We do have that cross section we created so let's turn that on and see what we can see.

Not bad actually. I think I'd like to have a little more clearance between the inside (purple) bezel and the top of the paddle (blue). I also want a bit more clearance between the slot (pocket) and the base of the paddle as the fit was a bit tight when I printed the last one.

Let's edit the paddle. The paddle parts are located in the "Enclosure Bottom" folder in the browser (no, not your web browser, the one on the left side of the screen LOL). Expand that to find the 4 paddles. Then activate SwitchPaddle:1. 2 thru 4 are copies and will update automatically. 

I also want to point out that when you activate a component... the timeline changes and shows you only the features for that specific component.

 ProTip: The Switch Paddles have a light blue vertical bar to the left and the timeline has a horizonal light blue bar above it. All components in Fusion are color coded.

OK, let's turn off some of the components that we don't need to see and get to work. Again... click on the eyeball to turn stuff on and off. When a component is "active" all other components become transparent. You can still click on them or reference them if you want to.

 The first sketch in the timeline drives the thickness of paddle so we'll edit that sketch. It's a very simple sketch where I just created a 0.2mm offset. I want to increase that offset but I also want to monitor the paddle thickness, so I'll create a reference dimension to monitor how the thickness changes as I modify the offset value.

Pro Tip: Reference dimensions are automatically created when you dimension fully constrained geometry, and you can right click any dimension and change its state from driving to driven at any time. Just know that you can't modify a driven dimension. Driven dim's are in parenthesis e.g. (2mm).

Ok. Looks like we have some room to make changes. I changed the offset to 0.35mm from 0.20mm. I hoping this is enough wiggle room to allow the blade to rock back and forth more than flexing because it's held tightly. We will see, I'm creating this as I make the edits. I also have a 0.4mm increase in thickness for the paddle as well.

OK, not bad, no blow-ups.

Let's modify the paddle height and make it a little shorter to get that clearance we need under the bezel lip. This feature grows up from the slot shaped base. The length of this feature is modified from the "extrude" feature and not from the sketch so let's decrease the distance 1mm for that extra clearance. It was 18mm and I changed it to 17mm

Let's accept and see how things are progressing.

Looks like 1mm is a bit much. I'll go in and change the distance to 17.5mm and that should be perfect.

Much better. My last edit to the paddle will be to move the little tab piece to the left a little. I have quite a bit of slop built into the assembly and it's on the close side. I don't want the paddle to bottom out on the bezel before activating the switch so I'll change that value real quick. For this one I need to edit the sketch. All I need to do is edit the 4.5mm dim on the top right and change it to 5mm and that should do it.

Perfect! That looks pretty good. I also added a chamfer to the inside for a little added strength.

I'm also going to move the surface under the paddle ~0.5mm just to be safe.

Again... to edit the bezel, we activate the bezel. I already have an offset feature in the timeline from when I modeled this, so I'll just edit that feature and increase the value by 0.5mm

 Pro Tip: You can see the highlighted feature in the timeline and also the faces that are associated with that feature. These are the clues that you need to pay attention to.

OK... That's looking good. I think that's it for the paddle refinement. Only one last challenge to tackle.

I'm going to close this post here and pick up the ribbon cable routing in the nest post.

See ya there. 

Edited March 7 by Penatr8tor
Misspelled some stuff

[claudermilk]

22 hours ago, Penatr8tor said:

Long ago, I worked for Racal-Datacom

Now there's a name I haven't thought about in a while! Also long agio I worked at a company that IIRC sold equipment to a branch of Racal. Small world.

That tutorial post is epic! Once you have reached a finished point on this little (snerk) tangent to your build diary, pulling these CAD tutorial posts out to a stand-alone tutorial thread would be great.

[Penatr8tor]

51 minutes ago, claudermilk said:

Now there's a name I haven't thought about in a while! Also long agio I worked at a company that IIRC sold equipment to a branch of Racal. Small world.

That tutorial post is epic! Once you have reached a finished point on this little (snerk) tangent to your build diary, pulling these CAD tutorial posts out to a stand-alone tutorial thread would be great.

Small world indeed.

Yeah, I was thinking that too. Shouldn't be too difficult to copy paste it to a new thread. 

I wanted to add that, a lot of times tutorials just run thru a build of some part or assembly as if everything just worked first time. Obviously not the case in the real world. The real world is messy and stuff doesn't always work. Focusing on work flow and the decision process to refine the design is more in line with how things go IRL. 

Edited March 8 by Penatr8tor
Added a topic

[Penatr8tor]

OK, Let's take care of the cable routing issue and see if we can't stick a fork into this design and call it done.

We need to get some real-world numbers on just how much the cable protrudes and whether or not we need to make the whole assembly wider. I installed the cable and measured how much of it protruded to get an idea of how much clearance I needed. Looks like 2mm is the minimum. I think 2.5mm will work without issue.

Next up is to open up the model of the display and add a cable. 

So, this is a good time to talk about what's worth modelling and what isn't because I could just create a quick cut in the bezel part and call it a day but... I have another one of these displays that will eventually end up going on my VzBoT so, it's worth it to me to finalize the display model so that I can use it on the next screen enclosure.

The modelling process is the same and I 'll just quickly go thru the steps. I think there may be a wire and cabling tutorial coming in the near future. Ya never know...

1. Model a rectangle the same size as the connector.

2. Model the flat rigid part of the ribbon cable (the blue end).

3. Create 2 sketches. These sketches are needed to create a sweep feature. The sweep command sweeps a section along a path so we need a section sketch and also a path sketch. The sketches are super simple. For the section sketch I selected the front face of the cable end and offset a line the thickness of the cable (0.18mm)  Pro Tip: Fusion automatically creates invisible sketch geometry around the perimeter of the sketch surface so, I don't have to draw or project any lines on the edges. I just need a line to split the rectangle that's already there. The path sketch was created by selecting the side of the cable end. I just drew a small arc then attached a larger arc and a straight line for the tail. Because the path is defining the inside of the cable path... I compensated for the thickness by reducing the 1mm arc to 0.82mm so that by the time I create the feature... the outside radius measures 1mm.

4. Sweep command. The rest is pretty self-explanatory, I selected the top half of my 1st sketch as my profile and the second sketch as my path. 

And that's it for the ribbon cable.

Let's save and tab over to our enclosure model and update it to see what blows up. Now that we have the enclosure model open, we see some warning signs. 3 yellow triangles with a "!" in the center. This is an alert telling you that something has changed and, in our case, it's the display. To accept the newly changed geometry, click the symbol in the upper right corner.

And.... It looks like nothing blew up and nothing changed or more accurately, the changes are probably hidden.

Let's create another cross section so that we can investigate. The process is simple enough, we click the "section Analysis" tool in the "INSPECT" tab and click on a plane that passe thru the area we want the section to be. In this case it's the XZ plane located in the Origin folder in the browser on the left. This plane passes thru the center of the model longitudinally. 

And there's where we're interfering...

Decision time: What are we going to do? I have a couple choices, 1. Cut a rectangular hole in the side or, 2. make the enclosure a little wider. I think in the grand scheme of things, a few millimeters isn't a showstopper so let's not cut corners and go with option 2.

Let's see if we can blow something up this time around 

Since the base plate drives the overall size of the enclosure, we'll modify the first sketch in the base plate component like we did last time. I'm going to just change the driving dimension to 5mm (was 3mm). This will change the driven dim's (fx:) to 5mm as well. If we find that it's too big... we'll go back and try something else.

And we finish the sketch and see what happens... And from the outside things look pretty good so far.

Let's check the inside by activating our section. I toggle visibility on (eyeball icon). If you have more than one section, you can expand the folder and select the one you want visible.

OK, not bad, we can work with this. I do notice that by making the enclosure larger, I'm also reducing the amount of overlap on the screen face. We need to modify that in addition to cutting away some of the bezel for cable clearance.

The base plate component does need one more change... I need to move the mounting holes up 2mm so that I can don't have to change and reprint the mounting bracket. Let's do that.  After finding the sketch that drives the mounting holes from the timeline, we right click and edit the sketch. I'll modify the 28.000mm dimension by double clicking and change it to 26mm. His moves the holes up so that the distance from the hole to the edge of the bezel is the same as it was before we increased the size by 2mm.

We finish the sketch and we're done.

We'll now create a cutout for the ribbon cable in the bezel part. We start by turning off the base plate so we can see where the cut out needs to be.

OK, this looks promising. All we need is a simple sketch with a rectangle and an extrude to cut away what we don't want. I decided that I want my sketch to start on the top surface. I could have started on the step below, but I want a little more clearance and that means cutting into the top a little.

Take a look at the above sketch, I used a "center rectangle", there are 3 types, corner to corner, center and angled. I like using the center rectangle because it automatically creates reference geometry for me. Once I place it... I can now constrain the center of the rectangle to the center of the object.  Pro-Tip: Without going into too much detail... sketch geometry needs to be constrained and every sketch should be constrained in two ways. It needs its boundary to be constrained and also, its location relative to its environment. That could be a component or the workspace origin. Nothing has to be constrained BTW, it's just good practice.

So, let's constrain our sketch. We'll start by adding a "Horizontal/Vertical" constraint. Constraints are located in the "CONSTRAINTS" tab. Easy enough, click the constraint and then click the center point of the rectangle and then the center point of the sketch. You'll see the horizonal constraint icon appear above the two points and now if you drag the sketch around you see that the rectangle can only be moved horizontally. Next, we add a few dimensions. 

Everything's constrained now. We know this because the color of all of the sketch geometry has changed to black. If it's black, it's constrained. 

Now we'll dial in the values.

OK, this looks good. Now all we need to do is finish the sketch and extrude.

Pro-Tip: I want to show you something below... Remember when I said that Fusion automatically creates invisible lines around the perimeter of a sketch when you sketch on existing faces? Because of this, I now have two profiles even though I only have one rectangle in the sketch. This occurs whenever your sketch entities cross over the boundary of the face you sketched on. This isn't something crucial, but it is something you can use in your favor on occasion so, keep an eye out.

OK, let's select the other side of our rectangle and extrude the two profiles together as one. 8mm looks like a good number. We're going to make sure we have a good amount of clearance. This is my 3rd time so I'm making sure this is the "charm" because, I'm going to have to reprint everything (with filament swap) except for the mount. (Which I find out later on I have to print anyways) 

Let's accept and inspect our results.

Looks like I have good clearance with the bezel.

and the cross section looks good.

And one final check to make sure we don't need to reprint the display mount and... looks like I'm getting really close to the table. I think we'll need to adjust the mount as well. I think we can just change the angle on the mount arm sketch to raise the bottom a bit.

And now to change the angle to 60 degrees and... Ka-Bleweeeeeey! Our first blow up.

What happened?

Let's explore.

I turned off the screen enclosure and the floor, so I only have the mount and screen. We also need to edit the mount model to determine what went wrong and how to fix it. I have always said, A good CAD person also needs to be a good detective. There are two ways to edit this model. 1. would be to open it up and edit it and the other way, 2. is to do what's called an "Edit in Place" this lets me edit a component in an assembly context where it's used somewhere else. That's what we're going to do and to so, we need to activate "edit in place". For this we click the little pencil next to the component name in the browser. Once activated we can edit to our hearts content and when we're done, we exit edit in place. Now, since we're editing a separate model from inside another model... the edited model won't be saved until we save the model that we currently have in session. We'll cover this again at the end.

OK, let's edit and explore.

If we look at the timeline everything looks good except for the two fillets near the end that are highlighted yellow. Icons in the timeline with a yellow background have issues, red background means it failed completely.

If you look at the end of the timeline, you'll see what looks like a black letter "T" with a fat top. This is called the "History Marker". We can move this marker by clicking and dragging along the timeline. It lets us insert geometry into the timeline. There's a lot we can do with the timeline but that's another tutorial. For now, we're just going to use it to step thru our design to find the failure.

Below I've right clicked on the sketch for the wing and if you look at the menu, you'll see a command called "Roll history marker here". Click that!

This is what happens. All geometry to the right of the marker has been turned off and is also greyed out. We can do whatever we want at this point, add fillets or draft or sketch and extrude, whatever... and once we move the marker back to the end... everything that we created is now inserted at that point in the timeline. Again, we'll explore this in another tutorial.

Let's use the controls located in the bottom left corner to step thru the timeline.

Ahhhh... that's what those are for. 

If you press the center play button it will step thru every feature like a video. The smaller arrows step one feature at a time and the outer most arrows take you to either the start or the end. For our exploration we'll use single step to move the marker forward (right) to see where our error is.

As I step forward, everything is good up to this one "delete face " feature.

Once I go past it... that's where it blows up.

So, let's look at this feature by editing it. Right click and edit the feature from the timeline, I'm sure you've got this by now so, let's see.

Well, I certainly don't want to delete those faces, so we'll back out and delete that one feature. You might ask why I had that feature in the first place. Delete face is a really good tool for getting rid of unwanted geometry. I probably didn't want those sharp tips poking out and when I changed the angle... the face I originally wanted gone is not there anymore, so the face I wanted to delete is now one I want. As if that makes any sense LOL.

So, now after deleting the delete face feature... we lost our fillets, and we now have those unwanted tips. We'll just create a sketch and do a cut extrude to remove them with a cut.

We sketch on the top of one of the wings and draw a rectangle. I picked the left-wing top as my sketch plane and made a corner-to-corner rectangle that's connected to the left edge. You can see that the left vertical line of the rectangle is already constrained because it's black.

Now we'll constrain our sketch geometry to our model. I'm just going to attach the corners of the rectangle to existing geometry by using the "Coincident" constraint. (menu at top middle of screen) Just click point to point.

OK, let's finish our sketch and do a cut extrude. We'll do a cut all thru the existing geometry and accept.

OK, that looks good. Let's add some fillets (remember as many fillets at the end as you can). And we'll move the timeline to the end and see how things look.

Fillets added and I also punched 3 holes thru the bottom so that I can run a hex key thru them so that I can remove the mount without removing the screen.

To exit "edit in place" we need to click on the green dot with check mark at the top center of the screen.

OK, Mission accomplished! Everything looks good, we checked all the boxes and now we'll export our models for print.

To export a model for printing we only need to right click on the part from the browser and select "Save As Mesh" that will bring up a menu with export options.

I have mine set to create a binary STL file in Millimeters with High refinement. There's also a check box that when checked Fusion will launch your slicer and load the file onto your build plate. I just save to disk but that's me. You have options, use them to make your experience fit your workflow. 

And there ya have it.

I will report back with a post once I have everything printed and we'll see if there's anything we missed in CAD.

Edited March 8 by Penatr8tor
Spelling of course