Help please

[TrainMaster]

I am, admittedly VERY new to this software.

With Fusion 360 becoming more of a licensing hassle, I'm trying new things. Also, I've heard that this is more like solidworks...which I'd love to get used to also.

But, I seem to be fighting with the software to just understand how to make things work. I started with a box, but can't edit it to remove the junk I don't want.

So, I followed a tutorial that suggested that I need to start with sketches. Okay..no problem....until I have an issue. Then, I seem to have to start all over...no matter what I do.

So...leads me here.... I've started this file 4 times. Because, everytime I touch the file, unless it's to add something new...I seem to break what's there and I cannot get it to recompute, redraw, or do anything.

I'm attaching a screenshot and the original file in hopes that someone can tell me that I've done something stupid and, actually, has a fix for it. The internet seems to be the who's who of tutorials for 0.17...but, I'm running 0.18 on Windows 10 or Ubuntu. Both have similar results...so...I know it's me!!! LMAO

Thanks for any help.

[chrisb]

Hi and welcome to the forum!

Your model is not so bad for a start. The issues you are facing are probably due to the "topological naming" problems which FreeCAD still has: You have attached your sketches to a face of the previous feature. When you change something from an earlier development step these faces can be renumbered which spoils your attachments. It is better to attach the sketches to the main planes if possible. For further explanations have a look at this page, especially the paragraph about creating stable models

You could easily achieve this by starting with a reversed pad and then place all further sketches on the main XY-plane.

Furthermore I strongly recommend to fully constrain your sketches. Have a look at the PartDesign Tutorials or at the Sketcher Tuorial to learn more.

[drmacro]

Welcome!

I know what you're feeling. I worked in the CAD world for 40 some years, taught, coded, consulted, and was an end user on Solidworks, AutoCAD, and a host of CAD software's no one remembers anymore.

When I picked up FC several years back I had the same feelings.

So what you're seeing is a common new user thing. First let me point you to this on creating stable models: https://www.freecadweb.org/wiki/Feature ... ble_models

That's got good info, but, the short of it is: there is a thought process and some "ways of FreeCAD" that experience teaches.

Then there is the why what you see is happening and how to make it better...some of which goes back to the previous sentence.

The novice (?) approach is to draw a rectangle in the sketcher (save the sketch, tip: rename the sketch to something memorable, get used to this step, you'll be glad you did ), pad it (name the pad), select the top face of the resulting slab, select "new sketch", and draw, for example, the holes as you did. Then pocket that sketch. Simple...two holes.

But, there's a gotcha. What this does is attach the sketch to the face, let's say FC calls it Face001. Now if Face001 never goes away or the name never changes, then the model will be fine. Unfortunately, when you cumulatively build the model (choosing subsequent faces and building on them) if you back up the tree and change something that triggers Face001 to be a different face, then the model breaks. (Now, i'm simplifying a LOT, so the gurus will most likely thrash me roundly...so, be it and I might learn new stuff.

Oh, and fully constrained sketches are always better, but, we all do plenty of experimentation with limited or no constraints. At least I do for concepts of the part, then commit full constraint later. This can bite you occasionally, so best practice is to constrain early rather than later.

So, the first thing I learned was to give a fair bit of fore thought to how I want the model to evolve.

If there are features that will change a lot or are parameterized (say for designing a project box that is always the same basic shape, but bigger or smaller) there are ways to use the spreadsheet workbench to drive the size.

If the feature is somewhat independent, then you can attach their sketch to plane (default, datum plane/edge, etc.) rather than the geometry created from some pad or pocket.

When you have, for example, a pocket that is relative to other features, you can, for example use a shape binder to bind to sketch geometry rather than faces whose names may change. (You could also use default planes XY, XZ, YZ, etc to attach to and make everything relative to 0,0,0. This might be ok for simple models, but, would probably get unwieldy quickly.)

That said...the changing internal face names gets better with each rev. If fact, I tried to break the file you sent in 0.19 on Ubuntu and couldn't
break it.

[drmacro]

And, while I was writing a tome, chrisb said it all much more succinctly.

[TrainMaster]

Firstly, thank you for not making me feel entirely stupid.

And...secondly, thank you for pointing me the proper direction.

I see that I have to "unlearn what I have learned" to quote a certain little green muffin man.

[chrisb]

Great post drmarco, I will refer to it in the future when it comes to explain why it is sensible to not attach sketches to faces.

[freedman]

My feeling is to place datum planes for every new face you want to work on. Here are some reasons why:

1) If planes get reassigned (by a topo error) you can highlight the plane in the tree and see stuff is in the wrong place, sketches don't give you that visual they have been moved.

2) Datum planes can hold multiple features so by refacing the datum plane (after a topo error) you can sometimes fix multiple errors with just one reface.

3) I think datum planes add some reliability to FreeCAD, since I started using them topo errors are almost non-existent.

Great post drmarco

+1

[wandererfan]

My feeling is to place datum planes for every new face you want to work on.

Should the act of mapping a sketch to a face create a datum plane automatically? Maybe hidden so it doesn't clutter the tree?
With a "show me my hidden planes so I can fix my model" button?

[chrisb]

That would be of no help. A DatumPlane attached to a face is almost as bad as attaching a sketch directly. DatumPlanes only show their advantage if they are attached to the MainPlanes - possibly augmented by Expressions -, or to Sketches or to other DatumGeometry following these very rules.

[drmacro]

That would be of no help. A DatumPlane attached to a face is almost as bad as attaching a sketch directly. DatumPlanes only show their advantage if they are attached to the MainPlanes - possibly augmented by Expressions -, or to Sketches or to other DatumGeometry following these very rules.

Agreed, if the datum is attached to a face that goes away, then it is pretty much the same issue as attaching the sketch to the face.

With the datum attached to MainPlanes, this should almost never happen. Though, if a sketch is attached to the datum, and, after some mod in the tree, creates a non-contigous solid the model engine will complain, no? (i note it does say "multiple solids not supported at this time", so maybe that might be ok in the future...)

I like the additions of datums and shape binders, as said these really help with tree stability. But, I have to admit, I find myself pondering when each is going to be most effective or best practice. (Spreadsheets and master sketches are useful tools as well...but, again, I find myself pondering which and when.)

Having come from a CSG background, I also sometimes go down the rabbit hole when I mix Part Desgin WB with Part WB Booleans.