Importing Autocad sketches into Solidworks

I have had this conversation before, but I think it was elsewhere.

I use AutoCad 2004 to create sketches, and then import them into Solidworks 2012, where I extrude them into shapes/solids, etc.

I have heard a lot of talk about how this is a bad idea, and SW sketch is better, but I would not agree, and as a matter of fact, I cannot do in SW sketching what I do in Acad sketching.
I have found SW sketching to be very clunky compared to Autocad, to the point where I avoid using sketching in SW unless I absolutely have to use it.

The problems that other's mention about importing Autocad 2D sketches into Solidworks just does not ever materialize.
Perhaps it is the way I do sketching in Autocad, ie: I generally draw past the end of lines, and then use the trim command, to get exact fits.
When I use OFFSET in Autocad, it is always an exact number.

One reason I import sketches from Acad to SW is that I use Autocad to rough out the basic engine geometry; it is like a sketchpad, often with several renditions of the same part.  Autocad is a great sketchpad, and it is very simple and fast to rough out geometry in 2D CAD in Acad.
Acad has very good grips, and an excellent stretch command, etc.
I can literally work 100's of times faster in Acad when doing 2D work than in SW, and I could never do production 2D work using a program like SW.
I have tried Draftsight, which is by the same folks who make SW, and it is a pretty decent 2D program, but still not anything I could actually use for production 2D CAD work.

I have my critical Acad 2D commands linked to keys on the keyboard, and so I use the keyboard in the left hand, and the mouse in the right hand, which is very efficient.
I center the critical Acad commands around the keys under the left hand, such as E, R, T, D, F, C, CC, V, VV, B, AA, S, etc., ie: line, rotate, trim, delete, move, copy, circle, offset, mirror, block, matchproperties, stretch, save.
The F8 key locks or unlocks ORTHO, and the F3 key toggles the SNAP to NODE functions on/off.
I don't use toolbars, icons, or pulldown menus, generally.
I litterally hammer my keyboard and mouse all day long, to the point where I have to wear a finger protector on my right index finger, to prevent wearing a groove in my finger.
The mouse is set up with the left button as enter, and also as repeat the last command.
Pressing and dragging the roll button pans on the drawing using the drag command.
I generally wear out about one mouse per year.

My work projects are all buildings and equipment shown in plan view.
I don't use paperspace, and I think paperspace is a bad idea unless you are doing something like airport work, in which case paperspace may be faster.
I use xref's, and insert them into modelspace, and size them using the XCLIP command.
My 2D drawings are a "what you see is what you get" arrangement.

When a project has hundreds of sheets, efficiency in 2D CAD means the difference between making the deadline, or missing the deadline, and also the difference between making a profit, and not.
I design as I go in Autocad, as if I were using a pen on paper.
Sometimes I insert entire libraries of previously designed switchgear, or even insert entire prevous projects, and then cut and paste from those drawings as needed to create new drawings/switchgear layouts.
I have not found a 2D program that comes anywhere close to being as efficient as Autocad 2004 for straight 2D CAD work.
If you don't use hotkeys on the keyboard with Acad, it is much slower.

I don't do anything to the 2D sketches when I import them into SW, as far as making sure they are fully defined, etc.
I just import them, and immediately do an extrusion, or cut, etc.
If I were doing machine design or something, I would probably pay more attention to fully defining things.
Ignoring the "fully defined" think in SW has never caused a problem, and I have created some pretty complex 3D models.

My approach is "don't fix things that are not broken", and "use the most efficient and fastest method that works for both preliminary layout/design, and 3D modeling; which is sketch in Acad and import the final sketches into SW".

Works very well for me.
I about gave up using Solidworks due to how clunky the 2D sketching was, and then discovered importing 2D sketches from Autocad.
If I had to use Solidworks only to do sketches, I would not use it.

Sometimes I use Solidworks if I have a lot of odd concrete slab elevations to deal with, and I am trying to turn feeder conduits out of the top or bottom of switchgear, and land within a narrowly defined range.

I also set up 2D sheets in Solidworks sometimes, by dragging a 3D model onto the SW 2D sheet.
This makes it very easy to generate isometric views of parts.
Sometimes I import the Solidworks 2D drawings back into Autocad, for reference, but generally don't use Solidworks 2D drawings because they are created from the 3D model, and curved lines and sometimes straight lines are approximated from the 3D model, and are often fragmented.
Fragmented lines are not usable in a 2D drawing other than in something like an isometric view.

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I guess I don't understand why you use SW at all. After you insert  your ACAD sketch you said you extrude it & maybe add some additional 3D features? Are you using the 3D model for printing or CAM? Or just making 3D views for your ACAD drawings? How complex are the sketches you use?

John

That is a good question.
I have used the setup for so long that I don't even think about why I do what I do these days.

Generally, I use a few photos of a known engine, such as the Baker Ball Hopper Monitor in my avatar.
I import the photos into Autocad, and trace over them to get basic shapes and relative sizes of parts.
If I can find a section of the original engine, like I found for the Ball Hopper Monitor in one of the Baker factory brochures, that helps a great deal in getting things accurate and true to the original engine design.
Also, if I can find someone who has an original engine, like I did with the Ball Hopper Monitor, I can get exact dimensions of the original parts, and that helps immensely.

Once the overall engine is drawn in 2D Autocad, then I start creating 3D parts one at a time in Solidworks.
The 2D drawings generally do not have draft angle, and so that is added as the part is extruded from the sketch.
The parting line has to be identified, and the draft angle has to extend out from the parting line.

3D modeling accomplishes several things.
It gives a good 3-dimensional image of how the parts will look, which one cannot get from a flat 2D drawing.
The parts can be assembled to verify that the fit is exact; verify that bolt holes and passages in adjoining parts line up correctly; verify that the rotating parts have sufficient clearances, etc.
And a motion study can be run in Solidworks, which allows the engine to operate virtually.
The motion study is very useful, since the motion study will not run if the parts are not correctly aligned/sized/assembled.
I generally add one part at a time to the motion study, and test to see if the study works.
If the study stops working after a part is added, then I know there is a problem with that one part.
If all the 3D parts are made before the motion study, and the motion study does not work, then it may be a needle in a haystack situation, finding out which part is creating the problem.  And correcting one part could then cascade errors to many other parts.
Each part needs to be tested in the motion study as it is made.

Then, in Solidworks, I add machining allowance to pieces that must be machined.
I can toggle the machining allowance layers on and off, so that it does not interfere with the motion study.
The motion study uses parts that are assembled as if they were as-machined.
The machining allowances are used in conjuction with 3D printing, to make patterns, with the correct shrinkage factor added at the time the Prusa slicer program is used.

So in summary, Solidworks is used to make sure things fit and move correctly, and also used to print patterns on a 3D printer.
The actual 2D drawings originate in Autocad, and remain in Autocad.
Isometric views are exported from Solidworks to Autocad.
It is an iterative process.

Sometimes the sketches created in Autocad are simple, and sometimes they are quite complex.
Much depends on exactly how you want to make your sketches, and the method varies depending on the part that is to be modeled.
Some parts lend themselves to a complex initial sketch.

It seems like Solidworks tried to come up with some clever tricks to make 2D drafting easier, and in some ways it does make 2D drafting easier, but generally the tricks get in the way, and are counterproductive.
The constraints that Solidworks adds to a sketch are can be a real pain to deal with, and are not necessary when you import a sketch.
I think Solidworks may use different 2D drafting methods to avoiding copyright infringement on Autocad.

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Edit:
You can see the process I use at this thread:
https://www.modelenginemaker.com/index.php/topic,11920.0.html

The spark plug sketch below that I made in Autocad was pretty complex, but easy to make in Autocad by sketching over 1/2 the photo.
The resulting sketch was easy to revolve in Solidworks, and while the 3D plug is not exact, it is sufficient for the use in the 3D model.

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CI, this thread from HMEM was the (long) discussion triggering my dejavu-all-over-again. The captured quotes in some replies make reference to GreenTwin & occasionally 'Pat'? but current member shows as user_45737. Is that you? Anyway, this Acad import to Solidworks subject was discussed at length. All I can say is if your unique workflow & methods & habits are working for you, that's great. Power to you. I can't contribute much over what was already posted there.

https://www.homemodelenginemachinist.com/threads/constraints-dimensions-or-no-constraints-dimensions-in-3d-modeling.34573/page-3

Quote from: petertha..... triggering my dejavu-all-over-again. The captured quotes in some replies make reference to GreenTwin & occasionally 'Pat'? but current member shows as user_45737. Is that you?

Maybe.....
Pat J/GreenTwin/Casting Iron/etc.
I quit HMEM, and got relegated to the lowly "user_45737", LOL.
You have a good memory.

I have posted a few places in the past.
Ended up here since this is the place to be.

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We have discussed this before.

What do you do when a part created from an Autocad sketch and turned into a 3D part in SW needs to be altered or a mating part gets altered?

Do you have to go back to Autocad, edit your original 2D sketch then import that again and create a new version of the 3D part?

Or like I get using just the one program if I change say the PCD of a bolt pattern on a cylinder then Alibre will automatically alter the cylinder cover's PCD to suit.

Or what if when you assemble the 3D parts and find they clash, can you directly edit the problem part in the assembly or do you need to go back to Autocad and make changes there

Here is a video I did for somebody last week, after the initial assembly I use the geometry from the cover to place the holes in the cylinder not a separate sketch. I then show how by moving the cover the holes move with it, I would get similar if I altered the PCD of the hole sin the cover with them also being carried over to the block,

https://youtu.be/oVx1Rzf5Vns?si=BA7PrQOUoP0CQ6B6

As said if it works for you then stick with it I know using the one program works for me as I get plenty of models made. On the odd occasion if I want to alter a part that was created in Alibre when doing the CAM in F360 it is a pain if I want to make alterations after exporting so would expect similar problems with your method.

Quote from: JasonbWhat do you do when a part created from an Autocad sketch and turned into a 3D part in SW needs to be altered or a mating part gets altered?

There is not really an absolute way I do everything; it varies by the part, circumstance, and engine.
If a part gets modified in 3D, then either a 2D sketch has to be generated in Solidworks and imported back to Autocad, or if the change is simple, then the Autocad sketch can be edited by itself.

If a part gets imported back to Autocad, one has to decide if the fillets need to be stripped off, since they are what cause a lot of line fragmentation.
The 2D Autocad drawings need to be clean and non-fragmented, if possible, else they get difficult to dimension and such.

Anyway, that is my method, and I use it for lack of a better way to do things.
It is not a perfect method, but it does what I need it to do.
The alternative methods mentioned just don't work for me, especially in the early phases of the design, where there is a lot of sketching and such to try different things, and look at them all side-by-side in 2D.
My 2D work in Autocad is like a computerized chalkboard, with lots of preliminary sketching.

Quote from: JasonbWe have discussed this before.

Yes we have, but I think some folks assume that there is only one way to make 3D objects using only one program, but there are definitely optional and sometimes better ways to do it all.
One has to figure out what works best for their modeling.
The term "better" is a bit subjective, and will depend on the application.

As I mentioned, I could not do what I do in 2D and 3D if I only used Solidworks, or not do it in a reasonable amount of time.
There is only so much time in a day, and I still work full time (probably 60 or more hours a week), so there is no leisurly modeling work for me; it has to be fast.
I am not a spring chicken anymore either, and there is only so much time remaining until I go to the great modeling workshop in the sky, or wherever I happen to end up (opinions vary, LOL).

Edit02:
I made a magazine article about the Dake steam engine, and used Autocad2004 for the entire layout.
It looked identical to any other magazine article.
I sent it to a technical website that publishes interesting things, and the person who operated the site said "We cannot publish your article; it appears as if you have stolen an article from a magazine somewhere".
I sent him the 2D CAD file that contained the complete article.
He said "Well I guess it all depends on how you want to fly it", referring to Autocad.

Sometimes people view things only through their own lens, but that often limits the vision of what is really possible.
I typically am given work projects that others won't attempt, either because the project is too dirty, too complicated, or because people just assumed that there is no way to do the project.  I have to think outside the box with pretty much every work project I do.  I work with continuous processes that cannot be shut down, or can only be shut down for a very short period of time.  People say "that is easy, just remove the old equipment, and install new equipment".  I wish it were that simple.

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As I said in the other thread post something here from Autocad that you can't do in solidworks, I'd be interested to see what and why not. Certainly overlapping lines and trimming or giving any feature a dimension is not a problem with Alibre or F360 and as F360 is an Autodesk product the same as AutoCAd then seems they should both work in similar ways.

From what I remember of the thread over on HMEM you seemed to be the only one using that method if it works for you great but the one program seems to work for everybody else in that long thread.

Fusion 360 was developed seperately from Autocad initially, kind of a ground-up restart. More recently they are getting them to have common look/feel and menu setups, while they are putting in a lot more features of CAM, electronics, sheet metal, etc into Fusion. I do wish they would stop adding new stuff long enough to fix the little GUI bugs that users have complained of for a long time. Still, I like Fusion a lot, though I don't have much experience with the other apps to give it a real comparison.

Quote from: JasonbFrom what I remember of the thread over on HMEM you seemed to be the only one using that method if it works for you great but the one program seems to work for everybody else in that long thread.

In an ideal world, one 3D program should be able to do anything and everything one wants to do.
The world is definitely not ideal, nor are many 3D programs.

I have pondered these things for a while.
I can only speculate about why.

I think most people have not used Autocad professionally for 30 years, and have not automated their Autocad.
Autocad right out of the box is not much better than 2D in Solidworks, but customized Autocad is a whole nother animal.
In the old days, we had drafting folks, who did all of the 2D CAD work.
It did not take too long to figure out that it is much more efficient to just have engineers design directly in CAD, and not have a drafting person introducing errors.
In order to make it in the business, and to do your own design and CAD work, you have to be very proficient and fast at 2D CAD in Autocad (or whatever program you are using).
I would guess most 2D CAD users are not aware of just how fast a fully customized Autocad 2D application can be, especially someone who only used 2D CAD on a hobby level.

It is not really a matter of whether it can be done entirely in a 3D program or not, it is more about efficiency.
My efficiency at making sketches in Autocad is at least 100 times more efficient than making them in Solidworks, perhaps even a higher order of magnitude.
There is no sense trying to prove a point, when that causes one to slow down to a snail's pace.
I am sure there are some who can work efficiently in 3D modeling only, but I can't do sketching there efficiently.

I tend to do a lot with 2D and 3D, ie: I not only make 2D drawing, and make 3D models with the correct draft angle, parting lines, machining allowanced, etc; but I also make patterns with 3D printing, and castings.
Whatever I do has to work across a pretty broad spectrum.

It is easy to point out examples of how it may be better to do all the sketches in the 3D program, but when things get very complex, that analogy breaks down, for me anyway.
There is really no "one size fits all" solution with 2D/3D work, at least not for what I do.
If I could sketch efficiently in Solidworks, I would certainly use it for that.
If Solidworks did not fragment their 2D drawings, then that would be a huge plus, and I would use Solidworks to make 2D drawings.
I use the methods that work well for what I do; I don't really have any other good options.
Reality (my realities anyway) have to drive the situation, not hypothetical ideals.
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So what you're saying is you do civil plan type work on a regular basis and are familiar with the techniques and continue to use them in spite of what SW has to offer. If that works, what can I say?

I've run autocad, microstation, f360. As a long time SW user you just need to get away from using techniques for Autocad and make the transition to SW. I can't think of a single thing that would be faster in Acad than SW. Of course I've been running SW since 98+. Currently running 2013, maybe upgrade soon. Hot keys are also available in SW. If you discount the effort to go back and forth, sure I suppose it makes sense? I had an F360 license for CAM last year and even that was painful uploading, updating if a change was made. The CAM part of F360 was easy, but trying to make any edits to the solid or drawing new was excruciating. If I was going to go forward with F360. I'd just stop using SW and make the jump. It would be painful for a while. I saw this happen at a company transitioning from 2D Microstation to Solidworks. The guys who struggled with SW just couldn't get used to the way SW worked or struggled to pick up new commands and techniques.

By avoiding the switch you keep telling yourself the old way better. Of course it is, you already know how to do that. "Think outside the box for every project", except committing to learning to use SW to your advantage? This isn't an attack, just an observation. Every technique you've mentioned I use on a regular basis in SW. You just have to change your mindset to understand how to make the most of SW.

Quote from: dieselpilotSo what you're saying is you do civil plan type work on a regular basis and are familiar with the techniques and continue to use them in spite of what SW has to offer. If that works, what can I say?

I've run autocad, microstation, f360. As a long time SW user you just need to get away from using techniques for Autocad and make the transition to SW. I can't think of a single thing that would be faster in Acad than SW. Of course I've been running SW since 98+. Currently running 2013, maybe upgrade soon. Hot keys are also available in SW. If you discount the effort to go back and forth, sure I suppose it makes sense? I had an F360 license for CAM last year and even that was painful uploading, updating if a change was made. The CAM part of F360 was easy, but trying to make any edits to the solid or drawing new was excruciating. If I was going to go forward with F360. I'd just stop using SW and make the jump. It would be painful for a while. I saw this happen at a company transitioning from 2D Microstation to Solidworks. The guys who struggled with SW just couldn't get used to the way SW worked or struggled to pick up new commands and techniques.

By avoiding the switch you keep telling yourself the old way better. Of course it is, you already know how to do that. "Think outside the box for every project", except committing to learning to use SW to your advantage? This isn't an attack, just an observation. Every technique you've mentioned I use on a regular basis in SW. You just have to change your mindset to understand how to make the most of SW.

I get what you are saying completely.
I think if I had started using Solidworks in 1995, I would be making an argument about how Solidworks is much better than Autocad.
But having customized Autocad since 1995, there are a huge number of time-saving customizations I would have to give up if I went entirely to Solidworks.

And then there is the license thing to consider.
I purchased both Autocad 2004 and Solidworks 2012 under a one-time lump sum payment, perpetual.
So while that cost me perhaps 6 grand total, in the long run the perpetual licenses have saved me a literal fortune.
I have a buddy who spends at least $1,500 per seat upgrade fee every year, and he has had to do this for years.

I think if you learn a native program, you will be most efficient in that program.
Sort of like learning a language; if you learn english from day one, you will be most proficient at english, and learning a 2nd language may not be easy.

Believe me, I have decided to "make the leap" entirely into Solidworks more than once, but reality always brings me back to Autocad for roughing out the preliminary design, and Autocad for the final 2D drawings.
I use Solidworks occasionally for work projects, and so my proficiency is limited by that.
I have used Autocad 2D for 30 years, almost all day every day, and my proficiency with Autocad is exceptional, especially as I mentioned with highly customized Autocad.

I really did not want to learn 3D modeling when I started to get serious in the model engine hobby (about 2009).
I cursed 3D programs, and was convinced I would never be able to learn them, much less use them effectively.
It took me a full year to begin to use Solidworks proficiently.
Conceptually, 2D CAD and 3D modeling are different universes.
My first 2D model engine drawing was total garbage.  Things did not fit; holes did not line up; rotating parts contacted stationary parts, etc., etc.
3D modeling is a superb design tool for engine work; there is really no parallel, and 3D modeling along with 3D printing has been a game changer in the hobby.

It is an interesting discussion I think from a standpoint of comparing how folks use these programs in the model engine hobby and the working world.




Edit:
The main secret to making Autocad fast is like I mentioned, program the critical functions so that you can use them with the index finger (or nearby finger) of the left hand using the keyboard.
This allows you to use two hands at the same time to draw, and you can focus on the work directly in front of you on the screen, and never have to look away to find a toolbar button or pulldown menu.
My wife said my autocad screen is just a blur of moving things.

Solidworks does allow you to set up shortcut keys in the same way, but I have never set that up in Solidworks.
If I were to set up identical shortcut keys in Solidworks that matched the ones I use in Autocad, that would be a huge improvement, but I would have to stop what I am doing to do that.

Another thing I do in Autocad that is not easy to do in Solidworks is that I create all of the drawings and sketches for an engine in a single file.
One has to be religious about backing up the file, since it is an "all the eggs in one basket" sort of thing.
By having everything in one file, I can pan around and see everything in a birdseye view, and copy, paste, etc.
For work projects, I often have 100 drawings in a single file, and I can see them all on the screen at the same time.
Again, it is all about efficiency.
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I had a boss at one company (one of many at different companies) who was right out of a Dilbert comic strip.
My boss had never done CAD work, but he was an "operator" if you know what I mean (a political player in the company).
He wrangled himself into the position of "Head of the CAD Committee", and proceeded to create the most moronic and unusable CAD standard you have ever seen.
He would state on one page how drawings should be set up, and then totally contradict that method a few pages later.

I confronted my boss about how his CAD standard was a huge pile of you-know-what.
He said "This is a secret document; how did you get a copy of it ?  We don't just give this out to anyone."
LOL, you can't make this up.

I told him that I could not follow his CAD standard even if I wanted to follow it, since it was garbage.
Needless to say we did not get along well at all.
My boss insisted that "engineers never do CAD work; only CAD drafting personnel are allowed to do CAD work".
I told him that it took 4 times longer for me to use a CAD technician than to just do the CAD myself, due to all the random errors that the technicians would introduce to the drawings.

So I used the CAD technicians only, and let them do all the CAD work, and I had to check and revise things over and over and over again.
Sometimes the CAD folks would change things that were originally correct to something incorrect.

I finally I told my boss that I would do my own CAD work, and if he did not like it, he could find someone else.
I have been doing my own CAD work ever since.

My boss did not care about having a good or efficient CAD standard; he only was in it to protect his "turf".
He told me "you are not on the CAD committe, and you will never be on the CAD committee".
It was a very exclusive club to be in.

It was with great irony that after several years went by, the company demoted my boss to just a standard engineer, and they forced him to do all of his own CAD work.
Poetic justice to say the least.
After 18 years of tolerating moronic (and some very good and smart) bosses, I flushed the proverbial corporate toilet, and started my own company.
In the 22 years of running my own company, I have never once had to do something that my moronic boss tried to make me do (sometimes my wife forces me to limit my junk food intake, so there is that).
I can do things more efficiently, and make a lot more money in less time than I ever earned in corporate, and the frustration level is perhaps 10% or less of what it was in the corporate world.

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Quote from: CIIt seems like Solidworks tried to come up with some clever tricks to make 2D drafting easier, and in some ways it does make 2D drafting easier, but generally the tricks get in the way, and are counterproductive.
The constraints that Solidworks adds to a sketch are can be a real pain to deal with, and are not necessary when you import a sketch.
I think Solidworks may use different 2D drafting methods to avoiding copyright infringement on Autocad.

There are copyrights on how to draw a circle or a line? Interesting theory. Autocad is an Autodesk product, the same company that owns/develops 3D Fusion360 & Inventor. SW came out in 95, 4 years before Inventor. If you ever tried F360 or Inventor I suspect you would see 99% exact same thing as SW - the 2D sketching tool is integrated within the 3D app & has analogous methods of defining & checking 2D constraints. From very limited exposure to OnShape, NX, SolidEdge, FreeCad, Rhino... they ALL have integrated sketch tools / module to then develop 3D shapes & surfaces. BTW importing is not limited to DXF/FWG from 2D CAD, many support vector files like SVG.

Nothing wrong with Acad, but sorry, they way you are using it within SW is just out of step with recommended methods & best practices. How its taught, how its used, how its supported, even how long you would last in an engineering office where your work was being shared or collaborated on with others. I suspect these factors don't really pertain to your personal situation as a hobbyist, but I'm highlighting this to others venturing into 3D who might be reading your opinions. You can haul gravel in a Porsche, but its just not that common.

BTW you mentioned what sound more like civil engineering work (vs aforementioned 3D modelers are more mechanical orientated). Have you checked into Revit (yet another Autodesk product). My civil eng & construction friends use it exclusively.

You most certainly could create all your sketches in a single file in SW, by starting with an assembly. I don't like working that way, but I use it during concept stages and for certain types of projects it's the best way to begin.

Most hobbyists aren't professional designers. It's something they do to burn some time or get away. Efficiency isn't a top priority. Most probably never get to the point where they are truly proficient. Much like a hobby machinist even with cnc tools in their shop couldn't grasp production machining in a modern shop. Where saving a second here and there in a program or tooling can add up to hours for a job.