Resize a STL File For Me

[MarkF]

Here are the Knob2 files for both the old 0.16 and the current 0.21.2 versions of FreeCAD.
These files have the dimensions for the D-shaft of 6.4mm diameter hole and 4.9mm flat
used in the last STL file I posted.

[bostonman]

Great, thanks again!

Hopefully your design will help others too. If all it needs is a few tweaks to resize the overall knob, then this could be quite useful to others since test equipment is prone to broken knobs.

This has certainly opened my eyes to being reminded of becoming more knowledgeable with 3D designs. What a great time we live in that helpful people can create something in one part of the country/world, send the file, and the end user can just print the part to fix their issue.

[bostonman]

MarkF,

I have a few questions but not sure if I'm going to ask them correctly. Since you created the 6mm shaft knob, referencing it may be the best way to ask my questions.

Basically I'm trying to expand my 3D modeling knowledge and using FreeCAD to do so. Much like other 3D models I've seen, you have several separate sections such as: Revolution, Sketch, Pad001, Sketch001, Sketch002, etc...

As I click on different sections of the knob, specific sections get highlighted. I'm curious why or when is it appropriate to create a separate sub part/section.

To be more specific, before I thought if I were to create a 3D model of a car, I'd create the body, engine, tires, etc... as individual pieces. What you seemed to do is create many separate pieces within just one part.

Recently I downloaded the STEP file for a BNC connector for reasons not worth getting into. The STEP file had numerous individual pieces all within just the BNC. So again, I'm wondering how/when this is done.

With your knob, as I click on each section, it gives me the impression numerous separate pieces were used, but I can't follow it.

Also, although I have several lingering questions I'm trying to work through with FreeCAD, one basic general question is say I wanted to add something like a plate for the knob to sit on. Let's say I wanted to make it a trophy. How do I make the plate "touching" the knob so it's all one piece that gets printed? I think this is called a face, but I haven't found any tutorials that explain this.

[MarkF]

I guess my first question is which version of FreeCAD are you referring to?

In the old version (discussed earlier), it is not possible to create multiple parts.

As far as order is concerned, in many times you don't have a lot of choice.
Certain operations depend of previous ones.  For example, you can't cut a hole in a part
you haven't created.  If you wanted to add a plate to the knob as you suggest, you would
just create a new sketch to the last operation in order to create a pad or perform a
revolution operation.  In the newer versions of FreeCAD, you can create multiple bodies
to build up your model.

The order you create the model depends a lot on what you're modelling.  Most likely, you
will build the model from the inside out.  Mainly you create a sketch, use that sketch
to perform a further operation (pad, revolve, cut), and then a boolean operation in some cases.
After you're comfortable, you can move to the 'draft' workbench to add text.  More advanced
operations to learn are the loft and pipes to create a curved surface or to draw a sketch along
a path.  In the beginning, you try to do things a certain way and find out you can't get from
point A to point B and will need to do it differently.  Especially in the older versions.
I do most of my modelling in the 'part design' workbench building sketch upon sketch.
Think of a sketch as the shape of the tool you will use to draw with.

I can suggest a few YouTube channels:
  - https://www.youtube.com/playlist?list=PL7eiW2bt21YU6QEbly78kUgQCNEiDUwSH
  - https://www.youtube.com/playlist?list=PLWuyJLVUNtc0UszswD0oD5q4VeWTrK7JC

Perhaps a photo of the two versions of FreeCAD:
 

[bostonman]

I watched some of those videos and will watch more as time goes on.

Recently I wanted to make a shape (using Free CAD v0.16) and attached a general sketch. In order to make this, I made the outside circle 50mm, the next one in 40mm, and then used pad to give it height.

After I added another shape making the circle 40mm (so it meets the previous circle), the inside one 15mm, and used pad to bring the height slightly less than the other shape.

Although the object came out correctly, I sense this isn't the correct way to do it; nor does the slicing software seem happy because it's doing some funky stuff with the layers. If I try adding a chamfer to the outside (higher raised) circle, the slicing software seems to not see it (even though I exported all the associated stuff in the left side panel).

I'm not asking for someone to create this, but only asking whether this needs to be done as two sketches, add something, or whatever, so I can learn. Keep in mind, I'm still trying to wrap my head around creating parts beyond a simple 2D sketch.

Also, I've yet to find why FreeCAD has a robot workbench. Does anyone know the reason for this? Although it's cool, I don't know what purpose it serves.

[MarkF]

I think the problem is that the inner disk and the outer ring are being seen as two different parts.
(i.e. the 40mm intersection is exact between the two.)
FreeCAD has some problems with exact edges like that.
You can try changing the inner disk to have its diameter equal to the diameter of the ring (i.e. 50mm or 40.001mm).

A better way of creating the part may be to create a disk with 50mm diameter with 20mm height and 15mm hole.
Then cut out the 40mm x 10mm hole from the inside.

[bostonman]

I think the problem is that the inner disk and the outer ring are being seen as two different parts.

From how I interpreted the image/stl, this was my thought too.

A better way of creating the part may be to create a disk with 50mm diameter with 20mm height and 15mm hole.
Then cut out the 40mm x 10mm hole from the inside.

I'll try this method tonight.

[MarkF]

I just recreated the part as you described including the chamfer without any issues in version 21.2
This might just be something that works better in the newer version of FreeCAD.

Like I said a while back:  "Sometimes you just have to tinker with how you create a part to make it work."


Also, I was able to create a STL and slice your zip file part without issue.
This also might be how the new version of FreeCAD creates STL files.


FYI: I'm using the latest PrusaSlicer on Windows 7.
I left Cura in the dust since they don't want to support Windows 7 any longer. 
Also, I hated the way you have to control Cura's view angle on a laptop without a mouse.
I wish both slicers would adopt FreeCAD's SHIFT/ALT pan and rotate control.

[bostonman]

I have a Win7 laptop as well that I can install V21.2 on.

Like I said a while back:  "Sometimes you just have to tinker with how you create a part to make it work."

I fully agree and it's why I tried making the second circle equal to the diameter of the other circle. In my mind, it didn't make sense because, as you stated, and I assumed, it's making two separate parts that "touch" each other rather than uniform.

My point is that I did spend time tinkering. In my slicing software, one view didn't show the chamfer, but the 3D view did, however, it also showed support material embedded in the inner circle; this is when it being wrong was obvious.

I attempted to print the part for fun, but it came out looking worse than expected.

[bostonman]

I'm uncertain whether I should start a new thread.

Periodically I tinker with FreeCAD (0.16) and trying to learn all the options. One option is the 'groove' option and I watched a video ().

Following the video to a degree, I managed to create a groove, but I don't understand what I actually did.

At approx. 2:40min into the video he creates a rectangle on top of the cylinder. First he created a cylinder, created a rectangle on top (for some reason), created the groove pattern, and then used that to make a 360 degree groove around the cylinder.

How is this different than using rotation?

Why was the rectangle needed?

Due to errors in my attempts, does the groove pattern need to be spaced a specific distance from the vertical axis?

It got somewhat confusing why another sketch was created, then pad was selected, another sketch, etc...  I managed to create a funky looking groove in my cylinder, but don't quite get the reasons for the steps including the last three or four steps after the groove was completed (and the rectangle was removed).

[MarkF]

How is this different than using rotation?
- The 'groove' tool basically does a rotation and then a cut.  It's doing multiple operations with one tool.

Why was the rectangle needed?
- The little rectangle on the top was to provide a reference face along the X-Z axis for the groove tool to operate upon.

Does the groove pattern need to be spaced a specific distance from the vertical axis?
- In this example, the 'groove' pattern will be revolved around the Z-axis.  So, you can't have any part of the pattern on the negative X-axis.  If you place part of the pattern on the Z-axis, the 'groove' tool will cut the object in half.

It got somewhat confusing why another sketch was created, then pad was selected, another sketch, etc...
- As mentioned above, the 2nd sketch and pad was to provide a reference plane for the 'groove' tool.  In the newer versions of FreeCAD, I didn't need to create that 2nd sketch.  I was able to reference the X-Z plane directly.  You have a more ways of creating reference planes in the newer versions.

[bostonman]

Sorry, I used the term 'rotation' and meant 'revolution' (located in the design drop down menu). At one point I tinkered with revolution, and, when I accomplished a groove pattern, wondered if a difference exists.

I was able to reference the X-Z plane directly.  You have a more ways of creating reference planes in the newer versions.

I assumed the groove "reference" was the vertical part of the groove pattern, however, if this is an outdated method and revised in later versions, no sense pondering on the topic.

[MarkF]

I don't know if there is a question there...

FreeCAD 0.16 was released in April 2016.
While it is terribly out of date, you still need to understand how
that version of the program works in order to be productive.
It wouldn't be important to others, but it's worth your time.

Let me pose a modification to the exercise in the video.
How would you rotate the groove pattern around the X-axis instead of the Z-axis?
I haven't tried this.

[bostonman]

How would you rotate the groove pattern around the X-axis instead of the Z-axis?
I haven't tried this.

That's a good question and I'm uncertain.

While I grasp some of the concepts, I don't necessarily understand the steps. At the end of the video he adds a sketch to the face of the rectangle, does something else, and makes it "vanish". Not sure why the rectangle sketch just can't be deleted at that point, however, my point is that it's a step I can easily follow but don't understand.

Per your question, a twist is: after making a cylinder, if I want to attach a square perpendicular to the cylinder, how do I attach the face? Each time I tried this last night, the square (or rectangle) would attach itself to the center of the x-axis.

[MarkF]

Not sure that I've figured out how version 0.16 is working.

However if you draw a cylinder around the z-axis as in the video.

Select the top cylinder end face as the reference to create the reference sketch (as the video).
Draw a square with two edges on each of the x-axis and y-axis in the positive direction.
Pad the reference square to a cube.
(Basically, make the little rectangle and pad in the video into a cube for more clarity.)

Now you have a cube which you can use to reference any of the faces in order
to create your cutting pattern.  The revolve then allows you to rotate the cutting pattern
in either the horizontal or vertical directions.

Clear as mud???   For me too.

To answer an earlier question, you can't delete this reference cube because that would
break the draw path used to update the part.  You can only add a cut of the cube at the
trailing end of the operations.

[bostonman]

I’ll tinker with it over the weekend.

Just for the record, I’m not necessarily trying to perfect learning FreeCAD, but more about trying to understand the foundation of it so I can understand what I’m actually looking at when I create a model. The goal and obvious method is to use the latest version rather than learn outdated tools, but I like learning the foundation rather than just steps.

[bostonman]

I hate to request another knob, but I tried tinkering with the design in v21 and can't figure out much.

Recently I purchased an Agilent 54831M scope with a missing horizontal knob (and broken shaft - something I'm in the process of replacing). I already have the same scope, so I'm able to measure the knob (and provide pictures which I'll post shortly).

I tried tinkering with the current knob design, but I couldn't figure out the tree structure. Is it too much trouble to edit the design (or create a fresh one if that's easier)?

You'll notice the face is slightly curved, but, I'm not looking for a perfect match, just something somewhat close. Due to the encoder being replaced, the current shaft size is a D shape and I've attached the dimensions from the datasheet.

On a side note, the knobs are slightly rubber type (I guess for better gripping). Does a filament exist that would be hard like PLA but slightly rubbery?

Edit: it would probably help if I included dimensions

base: 0.965" diameter
face: 0.9" diameter
length: 0.5"
little dimple on front: 0.38"

[MarkF]

Do you still want it in the old version of FreeCAD?

How many flutes (i.e. indents) are there on the outside?

How far does the shaft stick out from the scope face?
  (i.e. is the depth of the D-slot even with the scope face?)

[bostonman]

I'll count the flutes later.

The encoder shaft (as mentioned) is broken and replacements are unavailable. Someone on eBay is selling used ones for $92 (or so), but long story short, I found an alternate. The encoder leads need to be connected differently, and the only other difference is the shaft length.

From what I can tell, it's maybe 2mm shorter, but panel doesn't allow for the knob to go in any farther. The original knob D slot is flush with the back of the knob, so a 2mm shorter shaft shouldn't be a problem. If anything, I can (and probably will) put a dab of epoxy to hold it on.

It can be done in v21. My laptop runs that and I know it's easier.

[MarkF]

I have struggled with this one in version 0.16.
About ready to give up on the finger flutes on the outside when I thought of a new approach.
You should be able to open it in either version of FreeCAD.

Here is a version with 11 flutes you can have a play around with:
 - You can change the flute count by selecting the 'array' in the tree and changing 'number polar' in properities.
 - I just took a wild guess at the D-slot.  So, fix the dimensions in 'sketch002'.

[bostonman]

Thanks. I'll look at it later.

[MarkF]

I thought I would take this opportunity to create a teaching moment for anyone who would like to see how the knob was created.  This was done with version 0.16 of FreeCAD.  If using the newest version, you would probably do this with two bodies (one with the knob shape and another with the cutting objects).  Also as you do each step, FreeCAD seems to re-arrange the objects in the tree view.  I did screen captures of the final model.  So your tree will look different until completed.

Step 1:
  Create the knob profile and revolve it around the z-axis.  (via 'Part Design' workbench)



Step 2:
  Create and pocket the D-shaft hole.  (via 'Part Design' workbench)



Step 3:
  Create the cutting shape.  (via 'Part Design' workbench)
  Sketch, then Pad, then Fillet.



Step 4:
  Make an array of all the cutting surfaces. (via 'Draft' workbench)



Step 5:
  Cut the finger flutes into the knob.  (via 'Part' workbench)
  Select knob pocket, then cutting array, then cut.  (Windows CTRL+click for selecting multiple items in the tree.)



Step 6:
  Fillet the upper edge of the knob.  (via 'Part Design' workbench)
  Try to do fillets and chamfers as late as possible in the process.  Of all things they tend to break FreeCAD most of all.  You can not fillet or chamfer a distance greater or equal to the width of the surface.  Also if you modify an earlier sketch you will inadvertently change what edges are filleted or chamfered and will need to redo them to select the proper edges.

[bostonman]

I plan to look into tweaking this based off your feedback and tutorial.

As you mentioned, the tree structure seems to change in FreeCAD. Even though I've tinkered with FreeCAD several times, the tree structure is still challenging.

At the moment I'm dealing with a scope problem after reassembling, so tweaking and dealing with the knob is somewhat on the backburner.

[MarkF]

I noticed your other thread on replacing the encoder.  It looks like you're getting enough help, so I haven't been following it.

FreeCAD's tree is the mechanism for display/selection/edit of items. 
It is the basic flow of the creation of the model. 
You have little to no control over the order of those items.

How I navigate/use the tree as a novice (in no particular order):

• Show/hide the visibility of an item (click then space-bar).
  
  
• Transform a body (rotate and/or move)(right click).
  
  
• Change an item's appearance (color and transparency)(right click).
  
  
• Toggle 'active' body you wish to modify (if more than one)(right click).
  
  
• Double-click to edit an item.
  
  
• Create a 'link' (i.e. make a clone copy) of a body.
  For example, I created an HO scale office building.  The front, back, roof and one side wall were each a body.  I cloned the wall for the other side because both side walls were identical.  That allowed visualization of all sides while creating the interior.  Each body was then exported individually as STL files for 3D printing.
  
  
• Selection of items for export.
    Export to a STL file for 3D printing. 
    Export a STEP file for use as a model in PCB software or to import back into FreeCAD.
  
  
• You have a very limited ability to move a sketch from one body to another.
  

Create a separate body for each part of what you're making.  This allows you to place each in their proper location to insure that they match their counterpart.  For instance, a mount of some kind with multiple joints.  Each leg would be its own body with a joint at each end.  Then, you lineup the bodies at their joints.  You can animate the joints so the bodies can actually move but that's beyond my skill level.

I believe the 'body' was introduced in version 0.19.  But don't hold me to that.

The spreadsheet is very helpful too.  Instead of hardcoding dimensions, you place them in a spreadsheet allowing you to resize your model without the need to go into every place you used a particular dimension. 
I did a capacitor model and used a spreadsheet to define multiple capacitors for export.  See https://www.eevblog.com/forum/eda/tired-of-searching-for-basic-3d-cad-models/

[bostonman]

I'll tinker with this at some point. My goal was to reassemble the scope and tinker with the knob, but, after reassembling, the scope isn't working correctly. If things went according to plan, the scope would have been somewhat finalized and I'd be tinkering with the knob for ascetics.

BTW, the knob you made has a great height and width and both ends. I failed to mention this.