Resize a STL File For Me

[CatalinaWOW]

That is fine if you stop there.  But now imagine that you want to add cleats to the U.  By just padding a rectangle and merging it with the U.  Now the faces are different and it might make the reference go away.  But a different set of follow up operations would foul up a sketch tied to the base plane.


Again, I am a fumbler, not an expert, but the only way I see to know which way to go is to plan out the entire model, understanding all the pitfalls and decide then how to start.  Recognizing that if you change your plan in the middle you might need to go back and start over.  I am not proficient enough to do this so I do a lot of messing around a finding out, with quit a few dead ends and a few mysteries that have never been solved.

[MarkF]

There is no right or wrong here.

What you did is a correct thing to do.  What we are pointing out is that if, after the fact, you want to go back to an earlier step and make some change.  That change may break what you did in referencing the face.  There are ways to mitigate the risk of breaking the model while doing a modification.

You can reference one of the XYZ planes instead of a face.  However, this also has risks of breaking when editing older steps.

Only experience will determine which is best in any one situation.
Later, you will discover you can create custom reference planes in addition to the XYZ planes.

[bostonman]

I fully agree more than one way exists to do something; not just with 3D modeling.

Hopefully I wasn't coming off as asking for the 1-2-3 step process. Obviously the way I approached this design worked and various ways to create this exist. When the design "broke", I was unable to understand the reason(s) why and that was the more frustrating part.

I can always delete everything and return to just a single 'sketch', but I always look at such problems knowing a time will come when something is more complex, greater precision is needed, etc... and question the correct way to do it now before I'm confronted with such issues.

[MarkF]

I didn't think you were asking for a 1-2-3 step process.
And, I still don't know why your design broke.  Mostly, just guesses.

We're just pointing some of the pitfalls we have run across in our own designs and alternatives that may help you in the future.  I most cases it doesn't matter how you do the design.  The trouble starts raising its ugly head when you need to tweak the model.  Over simplified examples are your knobs and adjusting the dimensions of the hole for the D-shaft to correct for tolerances in the encoder and your 3D printer.  It's much easier to break a model if you need to add a hole or change a shape.

[bostonman]

It's nice to know that my confusion isn't just me.

I'll tinker with it more just for fun, but think the fillets is what added a layer of complexity and why things break when I tweak. I thought my foundation was enough to build on, but, after watching some of those FreeCAD videos, I learned lots exist I never imagined.

It's a comforting feeling though knowing something can be created and printed which makes 3D modeling so much fun.

[MarkF]

I was just sharing some new 3D designs for my model railroad.
Thought you might enjoy some more complex FreeCAD model examples:
(All the walls, roof, and furniture are their own 'body' in FreeCAD.)
   https://www.eevblog.com/forum/chat/model-trains/msg5697955/#msg5697955

[bostonman]

Wow, those are some great designs. Maybe you know FreeCAD better than you think.

[bostonman]

I have another design that went off into left field.

Attached is something I made for a project. The larger square began as 3.55" and the width of the two forks were 1.5" along with two ovals on the sides with pockets.

I wanted to increase the square to 3.6" and decrease the width of the forks to 1.4". After about three-hours of trying to accomplish this due to constraints getting in the way, I was successful, but realized one of the ovals went off into left field.

After I went back to the original design to tinker with the pockets. I discovered if I made pocket two 0" depth and pocket one "through", then it made pocket two a hole too.

My first question: why is pocket one affecting pocket two?

My other question: why did the oval go off into left field and how to get it back?

I thought trying to map it to a sketch would help or switching planes, but I don't understand what is going on.

As always, I'm trying to understand things rather than have it done for me.

[MarkF]

• In your "I'm More Lost" file you once again discovered what happens when you wipe-out a sketches reference.  I suspect FreeCAD changed the sketches name while you were making changes.  Sometimes it's easier to redraw a simple sketch rather than fixing its reference.  You can make this model by only referencing one of the axis planes.  I've attached an example.
  
  
• When making pockets, the sketch does NOT have to be on the surface.  It can be out in space as I demonstrated here.  Try changing the pocket to various distances instead of through all.  Also in your "I'm More Lost" file, you can see that your pocket is cutting into both forks.
  
  Review this video for "Understanding Pocket Types and Options"
  
  
  
• In both files, the sketch used for padding is not totally constrained.  Although this is okay to through something quickly together, it's a bad habit to get into.  It's also a possible source of things falling apart when later being edited.
  
  
• When constraining a sketch some things I noticed:  set opposite sides equal instead of their dimensions the same, set a line endpoint tangent to the axis instead of setting the distance to zero to attach a line to an axis.
  

[bostonman]

Sorry for the file naming. I was aggravated and named them out of being annoyed.

Am I suppose to select 'map sketch to a face' when I add something (in this case) an oval to make a pocket?

In the video you linked, he just clicked a face and selected 'create a sketch'. Maybe this is causing names/links to get renamed/break?

I never know how much to constrain. Usually I constrain lengths, I try making things equal so two sides move equally, etc... Eventually the design is full of so many constraints that I can't figure out which one is applied to which line(s).

Unless I haven't found it, I think being able to click on a constraint in either the constraint list or the image would help.

One minute I'm trying to change a line length and next minute fillets are giant reversed circles, some line changes length, a line goes off the main axis, etc...

[MarkF]

I couldn't care less what your filenames are.  They just give me a laugh.   

First, there should be a toolbar in sketcher with all the constraints listed.  It may be shrunk a little if all your toolbars are on the same line.  You can re-arrange them to suit.  If the toolbar is not there, go to View -> Toolbars and turn it on.



I tend to avoid mapping a sketch to a face unless it's needed.  It's has been the most likely way I've broken my models.  If you have something selected when you create a sketch, FreeCAD will use the selection as the reference plane.  Otherwise, it asks you which XYZ plane you wish to use.  I have a great deal of difficultly in fixing the reference plane after the fact.

I try to totally constrain my sketches.  Mostly starting with things vertical and horizontal edges.  Then constraining the lengths and diameters.  While dragging points, those large reversed circles and flip-flopping can be minimized by having more constrained prior to dragging a point.  You want to continue until FreeCAD tells you that there is zero DOF's left and the sketch turns green.

[CatalinaWOW]

I tend to use sketches for complex geometry, which means LOTS of constraints.  Naming the constraints can help in keeping track of them.  Also a large, high resolution screen so you you can see and separate them more easily. 

For simple shapes like ovals and circles I tend to use simple geometry from the Part Workbench.  I know many folk recommend not doing that, but it works for me.  As always you have to keep track of the geometry references.  The Body concept in Part Design handles much of this and is the reason that approach is recommended.  So far I haven't done complex stuff like multi-cylinder engines or submarines that really benefit from the recommended approach

[bostonman]

I couldn't care less what your filenames are.  They just give me a laugh.

Good to know, I'll keep up the good work. My PhD friend would name variables and such as 'dog', 'cat', etc... and I thought that was funny. Eventually I adopted it, so when I'm questioning a variable in something like an Excel spreadsheet, I'll use them.

The constraint list is visible on my screen. I do need to practice naming constraints as I go. Being able to click on a constraint and/or a line where it tells you the constraint number would help.

I'll also stop clicking 'map sketch to face' before adding a sketch. The concepts and planes I have an understanding of, but it's when FreeCAD (I assume no 3D modeling software comes without quirks) throws something off into left field, then I can't seem to connect my knowledge of X,Y, and Z planes, and what FreeCAD is torturing me with.

[MarkF]

The constraint list is visible on my screen. I do need to practice naming constraints as I go. Being able to click on a constraint and/or a line where it tells you the constraint number would help.

If I understand what you're saying, FreeCAD does do that.  All the constraints are listed in the 'Tasks' tab (mine is on the left bottom).  You can select one in the tab and it should get highlighted on the model.  The reverse is somewhat true also.  They are numbered at both places and you can delete one from both places.  I find it a little hard to select one on the model sometimes.

I have to check but I think some of them can be hidden.  Haven't really fleshed that out.

[bostonman]

I'll have to check again.

I thought when I click one in the 'tasks' tab, it doesn't highlight the line in the drawing.

All the constraints can be hidden at once by clicking the eye, and believe individual ones too.

[bostonman]

I have a few questions to (hopefully) get to another stage in learning/understanding FreeCAD. I know what I want to achieve, but not sure what terms to search for which makes it hard to search online.

To emphasize, I understand there is more than one way to do something and many tinker to achieve what they are trying to accomplish.

I don't necessarily have a particular project at the moment, but, to make my questions easier to visualize, let's say I want to make a box with two halves so the top can be removed and maybe four posts to use as legs. Again, this isn't an actual project, but the questions I have about FreeCAD are applicable to this example.

The main issue I keep having is: when I add a sketch (sketch 2) to the main sketch (sketch 1) so I can draw the circle for the legs, I can't work off the sketch 1 drawing. Meaning, I can't place a circle and then set constraints off sketch 1, I have to figure out where the lines are for sketch 1 and then set constraints off the X and Y axis.

Having said all this, my questions are:

Does a way exist to work off sketch 1 (it's visible, it's just unable to be 'touched' when in sketch 2.

When drawing the box, I'd start by making a square (or rectangle) and then padding it. How do I "cut" it to make it two halves, but also, the top (or bottom) half would need an inner lip to fit inside the other so they lock together eventually. So I'd need to work with one of the two sketches to add an inner lip, this is where being able to 'touch' sketch 1 would help.

Also, is there a way to set the distance between two curves? If I made the corners of the box a fillet, can I set the distance on the curves rather than the parallel lines? I find that when using fillets that the corners come out different lengths based on where you click on the lines. I end up trying to add constraints to them, however, all hell tends to break loose because it causes other stuff to fall off the deep end.

[rteodor]

Does a way exist to work off sketch 1 (it's visible, it's just unable to be 'touched' when in sketch 2.

Yes there is: while in "Sketcher" use "External geometry" to select whatever you want to import in the current sketch. This can be a feature (dot, line, circle) from a previous sketch or body. Of course it has to be made visible before. It is not possible to import external geometry from another body, (at least not directly).

When drawing the box, I'd start by making a square (or rectangle) and then padding it. How do I "cut" it to make it two halves...

As far as I know in "Part design" workbench is not possible to work with more than one solid object. Cutting a body in multiple pieces is possible in "Part" workbench, for example, by subtracting a proper shape.

PS: I use an older version so some things might have changed in the meantime.

[MarkF]

When drawing the box, I'd start by making a square (or rectangle) and then padding it. How do I "cut" it to make it two halves, but also, the top (or bottom) half would need an inner lip to fit inside the other so they lock together eventually. So I'd need to work with one of the two sketches to add an inner lip, this is where being able to 'touch' sketch 1 would help.

No.  You don't approach it that way.  You do it with two bodies.  One being the top half and the other the bottom half.  The two bodies are easier if they are both referenced the same way.  (i.e.  Pick a corner for (0,0) or I tend to make them symmetrical around the center of the box and specify a length and width.)  I also pick the divide between the top and bottom half as the XY plane.  The top and bottom height does not have to be symmetrical.

I just re-made a box for my handheld railroad throttles.  Looked at the attached for a blank box as an example.
You can make one of the halves 75% transparent to see how well they fit together.

Also, is there a way to set the distance between two curves? If I made the corners of the box a fillet, can I set the distance on the curves rather than the parallel lines? I find that when using fillets that the corners come out different lengths based on where you click on the lines. I end up trying to add constraints to them, however, all hell tends to break loose because it causes other stuff to fall off the deep end.

I would need an example, but you can probably use a tangent constraint so that the ends of the curve are 90 deg relative to the center.  Or you can use the vertical and horiz. constraints on the ends of the curve and the center point.  Also, if you're doing curves from within a sketch, you can use "End points and rim point" instead of "Center and end points".  Also, you can trim a corner using the "Constraint preserving sketch fillet" which leaves the corner as reference.

If your sketch falls apart, try constraining other parts of the sketch before the constraint that blows it up.  FreeCAD doesn't know what to do when a radius moves from the inside of a curve to the outside for example.  It tries to draw the curve the opposite direction.  Trying to draw close to the end dimension size helps.  Don't draw ten times bigger than actual size and expect good result scaling it one dimension at a time.  Other times it's better to draw some disconnected pieces and then with the "Coincident constraint" tied two points together after dimensioning.

I don't use the grid much anymore.  It might help you with an inch grid to get your zoom nearer to actual size before starting a sketch.

[CatalinaWOW]

First I will endorse all of MarkF's suggestions.  And add a methodology which helps getting the scale right in a great many cases.

Take a picture of whatever you are matching up with.  This doesn't help if both sides of all interfaces are from the ground up designs, but usually you are trying to make something that fits into the real world.  Sometimes a scanner is an easy tool for getting the picture, other times your cell phone or digital camera works.   Having a ruler (scale) or at least something of known dimension helps immensely.

Import and properly scale your picture and then draw your sketch over the photo.  FreeCAD 0.22 and 1.0 do this differently than earlier versions (much easier), but in either case there are excellent YouTube tutorials on how to do this. 

[bostonman]

I'll try all those suggestions.

I shouldn't have sent the message before giving more thought to all the questions I came up with over the weekend because I had one more.

When I use AutoCAD and need to do something such as add something that's both horizontal and vertical X units away, I'll draw a line from point A, go across X units and then up/down Y units. After I return and delete those lines.

Although maybe an easier method exists, it works for me, but is a pain to return to delete lines.

In the case of FreeCAD, I wanted to add something X and Y units away from a point, and did the same thing. I drew a horizontal line then a vertical, horizontal and vertical length constraints, added what I wanted, and then deleted the lines.

Does an easier way exist or is this the best approach?

My assumption is that I may throw FreeCAD off into a loop if I add lines and then delete them, but it didn't seem to have a negative affect.

[CatalinaWOW]

Everybody has their own way of seeing things.

In FreeCAD the concept of construction lines may help.  Draw the lines as you have, and identify them as construction lines.   They then won't be part of the model, though they are part of the file (that distinction is subtle, but important).  You won't need to, and possibly would prefer not to erase them.

When I am doing something like that I often just adjust the position coordinates of the object appropriately, or sometimes use the transform tool.

Both of these approaches can lead to a problem.  Due to rounding of the screen display the point you placed may not be identically equal to the location of an adjacent part.  The same to perhaps several decimal places, but not equal.  Whether this causes a problem or not depends on what downstream modifications you make.  A more robust approach is the external geometry approach mentioned above along with using the appropriate constraints in Sketcher (same, tangent or whatever).

[bostonman]

3D modeling isn't as easy as I initially thought.

I also have a 2D mindset where I draw a 2D box or whatever and pad it, so my lack of creative mind hinders me.

Each time I try to set a line to an external geometry it just gives me a circle with a line through it each time I hover over a line.

Attached is a picture of a concept I've struggled with. It's two shapes, but ideally it will be more elaborate such as the cylinder being a slot to hold a part and the rectangle being a mounting bracket.

The concept I've struggled with is: I need to make the rectangle "touch" the cylinder outside so it's one whole part. Both pieces will be different shapes/sizes, but they need to be one complete part in the end. My thought is to make the outside of the cylinder a geometry line and then use the tangent constraint to "touch" the two.

The other issue: the rectangle needs to be (for this discussion) centered. When I draw the rectangle, it starts off at 0.

[MarkF]

Not sure I grasp what you're trying to do here.

Maybe describe the drawing steps you're taking.

Notes:
 1)  To reference external geometry, the geometry must be in the same body.
     Not exactly.  There are other ways but I don't want to make it too complicated right now.

 2)  Just having the rectangle tangent with the cylinder is NOT good enough. 
     FreeCAD will see them as two objects which is not allowed at this time.
     They will have to overlap a little.  Even as much as 0.001" would be enough.

I'll wait till I understand better what the end product is to be.

[bostonman]

The drawing I provided is a rough idea to show what I was trying to learn, but let's say it's a cup holder with a wall mounted bracket.

The cylinder would be the cup holder part and the rectangle will be shaped into some sort of bracket. Both parts need to be as one, but, in my drawing, I just showed them with a large space for example purposes.

Can I just move the rectangle close to the cylinder (or overlap as you stated) and that will become "one" complete part? I assumed FreeCAD and slicing software would treat them as two separate pieces.

Also, as mentioned, I'd like to understand how to move the bracket (rectangle in this case) so that it's centered and not starting at point 0. Currently it's at the open end of the cylinder, but I'd like to understand how to make it so I can position the rectangle say halfway between both ends of the cylinder.

[MarkF]

Something like this?



Assume the cylinder is sitting on the XY plane.

Method 1:
Draw the bracket on the XY plane also and pad it to desired thickness.
Select the sketch with the bracket and change the Z attachment point in the "Data" tab.

Method 2:
Draw the bracket in the XZ plane at the desired profile.
Then pad the sketch with "Symmetric to plane" option selected to the desired width.