absolutely free CAD type programs

[ddmckee54]

I despise having to rent CAD software.

I tried FreeCad, there's a REALLY steep learning curve to it. I think this is partially due to it being an open-source product. Multiple people have designed different workbenches, and those workbenches often allow you to get to the same point in your design by taking different work-flow paths. To me, there are just too many ways to skin the same cat. You could watch a dozen tutorials to do the same thing by different people, and get about as many different ways to do it. It was just too confusing for me. Thus end-th the rant for the day.

If you are looking for a simple 3D CAD program that's FREE... 123Design, which was Fusion 360's predecessor, is still available to download at no cost. And from AutoDesk of all places, just Google "123design downloads" and you'll find it. It does not have any CAM functions, if CAM is what you want. I don't use it by the way, it didn't have all the features I wanted.

I opted to buy a perpetual license for Alibre Design Pro with the offline option. The offline option means the software doesn't have to phone home every 30 days to maintain an active license - unlike most other Cad packages. The perpetual license means that I OWN this software, and have the right to use it at the current version, from now until Hell freezes over. If, in the future, I decide to upgrade to the current version then I pay their yearly maintenance fee for 1 year and I can upgrade - no matter how many revisions occurred between my version and the current version. That yearly fee is about the same as what AutoDesk charges for a yearly subscription. The perpetual license cost is significantly less than the cost of just two years worth of subscription to Fusion 360. (I don't know, this might have been the 2nd rant for the day.)

The biggest downside to Alibre Design Pro is that it doesn't do CAM, but Alibre Design Expert does. When I get to the point I need that function I'll probably use FreeCad for that.

 

[petertha]

14 years later, I have never considered whether any sketch is fully defined or not.
I am told that I am doing it by default, but if so, I am not aware of what is happening.

If you are using Solidworks, 'fully defined' is certainly not the default. Only by adding constraints like dimensions & relations etc. does it become fully defined. This was no accident, they designed it this way. The sketch display even provides you useful visual color feedback as you start adding constraints: Blue = underdefined entity, Black = fully defined entity. You can verify this information in any SW training documentation. Its a core principle & gets discussed at the most basic level.

I think we have already talked at length about this, so no sense revisiting. But here is a recap.

- Will an underdefined 2D sketch still 'work' when used in a 3D feature like extruding or cutting or whatever? Yes it will. This is for a reason. You may presently know 8 of 10 dimensions in a sketch so you want that temporary flexibility to carry on. The other 2 dimensions or relations are to be determined later for whatever reason. The extrude wont fail as long as its geometrically compliant. SW will allow you to continue on.

- Is predominantly underdefined sketches considered good design practice? No. Because you increase the odds a feature will fail as part complexity increases. And when it does, finding the source & solution may not be easy for a number of reasons. It could be bad geometry, could be parametric dependencies. And this only gets worse as features cascade into parts and parts cascade into assemblies, design tables & other modelling features. A hand-drawn, unconstrained line at 89.9999 degrees looks remarkably like a fully constrained vertical line staring at the monitor, but it is not. Which is why SW colors it blue. This doesn't seem like a big deal but if some other feature requires it to be 'perpendicular to' or whatever, the math fails & Houston we have a problem.

- if I recall (and I may have this wrong), you are importing 2D sketch geometry from another app or source as opposed to drawing it as a native sketch within SW. This is fine, but for sure a much less common workflow. Its typically used when its easier to import existing 2D CAD work than reconstruct it from scratch with SW environment. This imported sketch may appear black (fully defined) but its really a special case. SW is trying to say 'its a group of entities that have relations between them as imported'. They really should have colored it purple to make this distinction, but they chose black because it 'kind of like' fully defined. Its more analogous to a Block where the sketch elements act as a group. They can be slid around or re-orientated as a group that still hang together. Or they can be exploded or de-constrained which is analogous to now underdefined. I'm trying to say this is a convenience, not necessarily a recommended practice.

I'm not telling you how to do things, but its also important to understand by & large how the app developers themselves are recommending best practice. Happy modelling!

 

[almega]

Which brings to mind an old CAD joke, I first heard back in the early 1980's:

God commands Noah to build an arc. Noah agrees.
A week later Noah has done nothing. God once again commands him to build the arc.
Another week goes by, Noah has still done nothing.
God, enraged by this, demands to know why Noah has not started construction.

Noah says, "But my Lord, I know not how. After all, there are 11 different ways to insert an arc!"

That's what we used to call a circle joke; you laugh when you get around to it.

 

[GreenTwin]

Thanks for the recap Petertha, I know we have discussed this before, but I must be honest, I still don't have a good grasp of it.

I started using Solidworks in 2012, and there were not many people on the forums using 3D modeling software, so there was not really in-depth discussions that I recall about the best way to do it.

I do generally import sketches from Autocad, because I find the Solidworks 2D functions to be extremely difficult to use.
Solidworks 2D is what I call "sticky", ie: every time I draw a line, SW tries to add all these relations, etc., and so when you try to adjust things, the entire sketch starts moving and stretching, etc.
So SW is trying to "help" me sketch, and basically getting in the way, and obstructing what I am trying to do.
Others say they really like the SW sketch functions.
I must say, I find the 2D part of SW almost useless, and it is horrible to try to use.
SW tries to make the difficult things easy, but in the process, it makes the simple things very difficult.

SW took the basic 2D functions from Autocad, and made them almost unusable, probably to avoid copyrights.
Autocad has very clear grips that can be sized or color-adjusted, and a nice ortho on/off snap.
The grips in SW really are terrible.
Grips are the thing I use the most, so it is critical that they be easily visible and work well.

I had the SW manuals, and I did read them, but they are very generic in what they cover, and as I mentioned before, they had no guidance as far as efficient approaches to designing engines.
Once I found out that my imported sketches worked well in SW, I ignored pretty much everything else.
I don't really like the dimensions to drive the sketch, and I find that most annoying.
The flip side is if I stopped and added driven dimensions to every sketch I did, I would run out of time and die of old age, since I do a LOT of sketches.

There are so many relations shown on the screen that I generally ignore them, ie: just sketch in Autocad and forget about keeping up with all that.
I suppose if I were doing commercial design, I would have to drill into the minutia of the "fully-defined" stuff.

Perhaps it is just me, but it is hard enough to focus on what I am trying to do with a design without deep-diving in to the layers of additional work that sketching in SW adds.
Its not like I have a lot of time for hobby work.

I do like to understand how I happened to stumble into the methods I use, and I like to understand why they work, and why they may not work.
I have actually never had a problem with a sketch, ever, and I do some pretty complex assemblies.
I can see where setting up driven dimensions with a spreadsheet could be very powerful, but my designs are not that cut-and-dried.
Luckily I can zero in on a good design pretty fast using my methods.

Occasionally someone mentions a new idea or method, and I try that, and it ends up causing trouble, either because it is not quite the right application, or I am applying it wrong.
I don't really stray much from how I do things in 3D.
Sort of like "If it is not broken, and it is working well, don't fix it".

I keep the "fully defined" stuff in the back of my head.
Perhaps one day it will click a bit more, and become clear as to how I could take advantage of that.
At this point I have no idea if something is fully defined or not, and I have no idea even how to go about making something "fully defined".
I think you mention that there are clues on the screen that will indicate that.

Anyway, thanks for the feedback/discussion.
I learn a bit about 3D every year.
I recall trying to draw engines in 2D, and having errors with holes lining up in mating parts, and dimensional errors between mating parts, etc., and I finally realized that I could get a much tigher/more correct design in 3D, and that is why I went the difficult route of learning 3D.
I consider using 3D simple now, and it is far simpler to use once you figure out how to use it.
I would never give up using 3D; there are too many valuable things that it does.

So I am not really promoting my method, but rather I just use what is most efficient for me.
I am perhaps 1000% more efficient with 3D when I import the sketches from Autocad.
I basically can't use SW without doing it this way.

Edit:
As a side note, my sketches tend to be rather complex.
I generally import raster images of real engines into Autocad, and then sketch over them, to get the basic geometry defined.
I don't know how to import a raster image into SW and sketch over it.
Seems like I have seen JasonB sketching over the top of a raster image of an engine.

Edit2:
For the green twin steam engine design, it was all developed from three photos, and so I imported the three images into Autocad, drew a grid over them, and then came up with proportional geometry.
Turned out to be a pretty accurate method, once I figured out how to compensate for a skewed photograph.
.

 

[petertha]

I don't know how to import a raster image into SW and sketch over it.

SW handles this readily. Not just the basics like image import, setup, orientation, dimensional scaling... You can even optionally have it determine outline sketch geometry to save you constructing by hand. But (like any app) lots of caveats here. The picture has to be clean & minimal contrast & distortion otherwise the advantage of auto pilot can be garbage in, garbage out syndrome.

Some YouTubes (there are many)

 

[petertha]

Solidworks 2D is what I call "sticky", ie: every time I draw a line, SW tries to add all these relations, etc., and so when you try to adjust things, the entire sketch starts moving and stretching, etc. So SW is trying to "help" me sketch, and basically getting in the way, and obstructing what I am trying to do.

Getting off topic but hopefully you are aware - its just a button click to turn relations on & off (the green boxes). Generally I draw without relations so its cleaner. The 'helper geometry' you are referring to can be utilized or ignored completely as you draw, its practically seamless. You are in the drivers seat. But OTOH at times you really do need to see or validate relations of your sketch or any element within it, so click them on temporarily & confirm. Its really that simple.

Using my previous example, if you drew a line at 89.99999 degrees because your hand-eye-mouse wasn't so accurate in that particular moment, SW will accept that odd angle no problem. But wouldn't you really want to verify its truly vertical by having it convey a [bar] symbol? This may seem nit-picky but when you extend the concept everything a sketch is supposedly defining - without relations how do you really know your bolt hole positioned is relative to an edge? Or its diameter is what you intended? Or it matches a hole on another part? The whole design process becomes one big 'I hope its OK guestimate'. This completely bypasses the power of CAD.

Anyway, back to the relations & heads up display & default dimensions & all that good stuff. You can save whatever preferences you prefer in templates. Every time you start a new part, pick from any number of custom templates.