Constraints/Dimensions or No Constraints/Dimensions in 3D Modeling

[johnmcc69]

No nothing blows up.
There seems to be a general misunderstanding about this.
The 3D program has no idea if you have imported a sketch from AutoCad or elsewhere, or whether the sketch was created in Solidworks.
It is just lines, endpoints, lengths and angles, in the Solidworks database.
There is nothing in the SW database that says "this line was drawn in AutoCad".
A line is a line.

Any changes that need to be made to a sketch can be made directly to the sketch in Solidworks.
Sometimes I erase a sketch in Solidworks, and copy and paste an entirely new revised sketch in its place. No problems doing this.

There is no reference back to a 2D program; I keep hearing this over and over, and it is false.

You make the initial sketch in Autocad, copy and paste it into Solidworks, and extrude your shape.
You can do this for every sketch you add in the Solidworks model.
Any tweeking to the sketch can be done in Solidworks, or as I mentioned you can copy/paste over a previously copy/pasted sketch.

Solidworks does not know you are importing sketches instead of creating them in native Solidworks.
Solidworks does not act any differently if you import all your sketches or create all of your sketches in Solidworks.

With all due respect, clearly you have no concept of what is happening with the sketch import feature, or what is happening in Solidworks with or without imported sketches.
Jason keeps repeating the same false things too, so clearly he is not understanding the import process or how it works either.

I mean, it is one thing to not recommend something because you fully understand how it works, but to not recommend something, and then make a series of false statements, is not really a recommendation based on facts.

No slights are intended towards anyone, but I can see this conversation is getting nowhere, and there is no understanding of what I am doing with either AutoCad or Solidworks, or what the programs themselves are doing.

I am going to throw in the towel on this discussion; it appears hopeless.

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Yes, I understand your frustration, BUT...

The whole point of what myself (& many other users here) are saying, is that you DON'T need a "Secondary" CAD tool to achieve what you're doing. Like mentioned (many) times before, the sketching tools in the 3D CAD program are VERY good. I can't understand why you import sketches...maybe you can post a screen shot of the types of sketches you import?

Like Peter mentions, when I have tried to import a sketch (to save a little time, I'm lazy sometimes..), it will "Blow up", end points aren't closed, polylines are a problem, "UNCONSTRAINED geometry", unclosed sketches...
I spend more time trying to fix these issues than it takes me to recreate it in the 3D sketcher.

Your method DOES work, but why not use the tool that is already built into the program??

Don't "Throw in the towel", these posts have some very good points about how to use the software. Like you said, this works for you & it is important that users realize that this is an option to use. There may be some crazy reason why your option maybe the only one. I've seen stranger circumstances..

John

 

[petertha]

The 3D program has no idea if you have imported a sketch from AutoCad or elsewhere, or whether the sketch was created in Solidworks.
It is just lines, endpoints, lengths and angles, in the Solidworks database. There is nothing in the SW database that says "this line was drawn in AutoCad".
A line is a line.
Nobody is disputing this. Nowhere have I said this is the case. Go back & read my posts carefully. Anyway this is not the point I'm trying to express. Your workflow works, but only to the extent of your current models. If you choose to expand your SW proficiency to the extent of its more advanced capabilities it has to offer, the likely hood of problems is higher with this workflow.

Any changes that need to be made to a sketch can be made directly to the sketch in Solidworks. Sometimes I erase a sketch in Solidworks, and copy and paste an entirely new revised sketch in its place. No problems doing this.
Nobody is disputing this. You can import a sketch, you can modify the imported sketch, you can use a portion of the sketch & delete the rest & you can draw a new sketch from scratch. The net result is a sketch. What I am talking about is relative advantages of sketching with SW.

There is no reference back to a 2D program; I keep hearing this over and over, and it is false.
Lets clarify this statement. You import a 2D sketch, no alteration, extrude it & now have a 3D model. OK. You open up the 2D model and change a dimension. Does SW know about that change & update accordingly? No. If you rename or delete the entire 2D file does SW know about that & change? No. Now the reverse. If you modify a different dimension within the SW sketch the subsequent extrude steps responds directly to that change, does the 2D program know about that & adaptively change? No. Conclusion: there is zero connectivity between the 2D & SW apps. The only time there was brief connectivity is when you manually pasted it in. The point is, this paste-in workflow just destroyed the entire concept of parametric design within the SW app which is foundational to not just making simple features but everything down the line including file management. Because the normal way to design is to have the capability to go to any sketch or feature within the tree & alter it.

Think about this in parallel terms of assemblies. Your assembly contains 2 parts, A & B. You go back & change part A, what happens in SW? The assembly immediately reads the current part A & refreshes itself with that change, which is exactly what we want. There is connectivity between the assembly and its parts. So going back to your 2D workflow by analogy, there is no connectivity, no automatic link. You must manually repeat the process: open up 2D, make a change, paste it in the right place...

You make the initial sketch in Autocad, copy and paste it into Solidworks, and extrude your shape. You can do this for every sketch you add in the Solidworks model. Any tweeking to the sketch can be done in Solidworks, or as I mentioned you can copy/paste over a previously copy/pasted sketch.
Solidworks does not know you are importing sketches instead of creating them in native Solidworks.
Solidworks does not act any differently if you import all your sketches or create all of your sketches in Solidworks.
All true, never disputed, but again, is not the point

With all due respect, clearly you have no concept of what is happening with the sketch import feature, or what is happening in Solidworks with or without imported sketches. Jason keeps repeating the same false things too, so clearly he is not understanding the import process or how it works either.
I am going to post a pictorial example. If it resonates with you, fine. If it doesn't that's OK too. I'm throwing in the towel after this.

 

[petertha]

My crude example. I just pulled some random 3D part to demonstrate a particular aspect of sketching based on bottom up geometric features. I numbered the screen grabs in sequence, hopefully makes sense. The takeaway point is you could do this with 2D cut & paste workflow, and it might not blow up, but it doesn't look like much fun to me, especially if there are going to be design changes. And there are always design changes.

1) random 3D part
2) I need an important reference point which is dimensioned relative to origin, required for following step. Select that plane & draw dimensioned sketch
3) I am making a plane in 3D space defined by 3 points, one of the points is utilizing a point from preceding step 2) the other are point features on the part itself
4) shows the fully defined plane based on aforementioned selection
5) draw a sketch on this plane. Make the hex shape, dimensionally offset & angular rotate from different features relative to underlying part
6) extruded cut result. Its entering the body at that weird angle
7) design change now, modify the base diameter of the part , click feature open sketch, changed base diameter from 4.0 to 4.5"
8) notice where this changed occurred, way up in history tree
9) resultant change to 3D part. A single dimensional change (7) cascaded through all the subsequent steps & made a new part obeying all the in between steps & constraints

Now take this sequence & evaluate all the different interaction steps between a separate 2D app vs SW. How did 2D know about those positions defining the plane reference points? It didn't. How did 2D know the correct orientation of the 3D plane ? It doesn't. What happens if you make a simple change like step 7) which can affect any number of inter-related features downstream? Or if the history tree is 500 steps long. Or maybe step 7 is not an error, you have 10 different configurations of this part all with slightly different dimensions. Rather than a button click refresh where al the dimensional attributes update themselves, my view is that you essentially start all over again with the separate disconnected 2D tool because it has no understanding or history of the 3D model. Can this process be done by 2D sketch pasting? Yes/Maybe. Is it time efficient & serving to reduce potential domino effect problems? (the bane of 3D modelling). IMHO the answer is No.

 

[Jasonb]

John post#5 has an example of what Pat imports. This looks a very simple item to sketch within most modern 3D programs and any changes to any feature along that shaft profile will simply be a click of the displayed dimension on the screen. Maybe Pat can attach that file or a dimensioned 2D drawing in pdf format so we can draw it in our individual ways and then use it a san example of how constraints and having the sketch created within the 3D program is advantagous for us.

I know PAT has said he NEVER has to change a sketch, he must be the lucky one as I don't feel that is normal either. I'll often need to tweak parts as an assembly comes together say change the length of a piston rod so I get equal clearance both ends. I also often make slight alterations as I build my models so go back and alter the 3D part, maybe as Pat has not actually made most of what he shows that is not yet an issue for him.

I often use features of a developing part to ref a new sketch from such as having a boss concentric to an earlier drawn round feature. How would you deal with that if the sketch has to be done elsewhere and then imported?

 

[Jasonb]

Pat post #203 you say you never have to go back and revise a sketch

Yet in post #219 you say you do revise sketches and import them again

So which is it you do? It's hard to reply when the facts keep changing

 

[Jasonb]

here is a good example of why sketching in SW, Alibre, etc can be of benifit compared with importing a 2D file from elsewhere. I am using a snip from Pats post #8

Pat has imported that blue profile from Autocad, I would simply draw it on a plane in Alibre. If I subsequently alter the previous features that make up the beam such as change th ewidth of the beam or the boss as shown with the red arrows I won't have to alter the blue sizes/positions/dimensions of the blue arrowed parts of the sketch as I can constrain them to those previous features.

At the very least Pat would have to go back and manually alter those two blue bits manually in SW

 

[GreenTwin]

Jason-

You are spinning my words like a top.
I have explained what I do numerous times.
Either you understand it, or you don't.
I am not going to keep repeating the same things over and over.

Its really simple.
1. Create the sketch in Autocad.
2. Copy/paste the sketch onto the Solidworks sketch plane.
3. Extrude the shape.
4. Tweek the sketch in Solidworks if desired.
5. If a major tweek is required, I generally go back to Autocad, and re-import the entire sketch, deleting the old sketch on the SW sketch plane.
I very seldom replace the entire sketch, but occasionally I do.
Generally I just tweek the sketch in Solidworks once the solid has been extruded.


After thinking about why I use AutoCad to created sketches (I never really ponder why I do it the way I do it), it now occurs to me why I use AutoCad to generate sketches.

I import photos of old engines into AutoCad as a raster image, and trace over them.
I don't know if Solidworks has the raster image import feature, or if it does, I don't know how to use it.
AutoCad is a good program to sketch over raster images, and it does not insert unnecessary stuff like relations, so you can create a clean and simple plain vanilla sketch that works well in Solidworks.


I had to load my Solidworks program on another computer, and so it is separated from my video screen recording program, else I would just make a screen video of what I do, which would probably save a lot of discussion.

I think Jason mentioned that he can import a raster image into Alibre, and he basically does the same thing that I do, which is trace over a raster image to create a 2D sketch in his native Alibre.

I will try and find a new screen video recorder for my Solidworks machine.

I think we are winding down this thread, and all very good points from many folks, not all of which I totally agree with, but good food for thought.

.

 

[GreenTwin]

One feature that I use a lot in Autocad is splines.

I find the spline function in Solidworks very hard to control; its like it has a mind of its own, and it keeps trying to snap to places that I don't want it to snap.

In Autocad, I can turn off the snaps entirely, which gives a very fine control over spline point placement, and I can't do this in Solidworks.

And the points along a spline don't drag well in Solidworks, and this is a big problem.

So with this single command, a spline is simple to accurately create and control in Autocad, and not easy to create accurately or control in Solidworks.

There are many similar commands that are very easy to use in Autocad, and not so easy to use in Solidworks.
The snaps are far more visible and usable in Autocad than Solidworks.

If I had to use the 2D features of Solidworks to make a living, I would go out of business in about 1 day.

I tried Draftsight, with the idea that I may replace Autocad with Draftsight.
Draftsight is pretty close to Autocad2004, but again, it is just different enough that I could never use Draftsight to make a living doing 2D work.

I am sure this point will be debated, but AutoCad2004 is many orders of magnitude more efficient at 2D work than Solidworks is at 2D work.
I have used both programs for years, and there is no comparision between 2D in Autocad and 2D in Solidworks.

One thing I have noticed about Solidworks, and this is just my opinion, is that it makes the simple things (like 2D sketching) difficult, and the difficult things easy.

For a beginner who is doing pure 3D modeling work with a single program, of course all of this discussion is just blah, blah, blah.

From a speed perspective, with me doing 2D work, Draftsight was about 50% the efficiency of Autocad2004, ie: my work speed dropped by 1/2 despite my best efforts to automate Draftsight.

Comparing the 2D function of Solidworks with the 2D function of AutoCad2004, my 2D work in SW is 1/20th the speed of my 2D work in Autocad.

If for no other reason, the savings in time I realize by using Autocad for most 2D sketching is what allows me to efficiently create a lot of 3D models.
I would never have been able to create the 3D models I have created in Solidworks only; no way.


.

 

[GreenTwin]

my view is that you essentially start all over again with the separate disconnected 2D tool because it has no understanding or history of the 3D model. Can this process be done by 2D sketch pasting? Yes/Maybe. Is it time efficient & serving to reduce potential domino effect problems? (the bane of 3D modelling). IMHO the answer is No.

And so my point is after I create the initial sketch in Autocad, and import it into Solidworks, I don't go back to that Autocad sketch again, unless like I detailed in the posts above, I want to do a second copy/past on the sketch (but it is very rare to have to import a sketch twice).

So basically the Autocad 2D sketches become disposable, and are not used again for anything.

The final 2D drawings are created in a Solidworks drawing file, and then exported back to an Autocad2004 DWG file, which creates the working drawings.
I would leave the working 2D drawings in Solidworks, but again, Autocad is so much easier as far as manipulating borders, arranging drawings, etc. that I always export 2D back to AutoCad.

I very often use an existing sketch in Solidworks to create a new sketch, by tracing over the old sketch that is on another sketch plane.
I change the model to wireframe to do this, and so all of my holes always match with mating parts.
I can also toggle on and off the view of sketches, and turn them on if I need to trace over one to match its size and location exactly.

I think my 3D models for the most part act just like your 3D models, without the driven/driving sketches though.
I would say that if you were to pull up one of my 3D models in your 3D program, in a blind test, you would never know it was not completely created in Solidworks.

you essentially start all over again with the separate disconnected 2D tool

No, I never start over again with a separate disconnected 2D tool.
Tweeking a sketch by whatever means is not starting over again by any measure.
There is never a scenario where I have to start all over again because I create sketches and import them.


Your example above, while valid, is not an old engine, and old engine reverse engineering is probably not so cut and dried as your example, at least I don't find it to be.
I change shapes such as circles by either scaling the circle up or down, changing the circle size in the dialog box, or more often just drawing a new circle and erasing the old one, but never by driving or driven dimensions.
Sometimes I do have to shift things a bit as I go, but that is generally minor alignment adjustments, not blow-up stuff.

One point of confusion may be that the approach one would use to design a new part from scratch, for a new device, is not necessarily the same approach as one would use when reverse-engineering an old engine or old drawings. At least that is my feeling about it.

There is a bit of an art to using 1840 drawings accurately, or to use photos only, but I can do that very easily in AutoCad, and not very easily at all in Solidworks.

.

 

[GreenTwin]

I think we have pretty much beat this horse to death.

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[Bazzer]

GreenTwin

I think you might have covered this, but I would say that creating the sketch in a 2D programme does create extra work if modifications are required.

I completely understand your workflow and I occasionally use it for importing unusual sketches that already exist, it is not my default method though as I find that the 3D CAD programmes have powerful sketch editing features without the need for another 2D CAD programme (Autocad or similar which of course I have).

My hat goes off to you for the nice 3D CAD models that you create but as you mentioned that is only the start of the process of making anything.
B.

 

[GreenTwin]

I think you might have covered this, but I would say that creating the sketch in a 2D programme does create extra work if modifications are required.

Not really, because almost always you tweek a sketch in Solidworks after you import it in, and you don't normally have to go back to Autocad and re-import.

I normally just make small modifications to the 2D sketch directly in Solidworks.

I completely understand your workflow and I occasionally use it for importing unusual sketches that already exist, it is not my default method though as I find that the 3D CAD programmes have powerful sketch editing features without the need for another 2D CAD programme (Autocad or similar which of course I have).

Jason makes a good point in that most hobby folks only have a single 3D program, and so importing 2D sketches is not an option.

My hat goes off to you for the nice 3D CAD models that you create but as you mentioned that is only the start of the process of making anything.

Thanks, I really like this hobby, especially when combined with the backyard foundry hobby.

Even JasonB is "going foundry".
So now that Jason is "going foundry", then the rest of you have no more excuses, so get busy on building that furnace.

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[Jasonb]

I very seldom replace the entire sketch, but occasionally I do.

That,s different from Never unless Solidworks defines Never differently

And now you tell us that once you have the 3D item complete you export back to Autocad, again loosing that parmetric feature that if anything is changed on that component or assembly then the working drawings will automatically update, no wonder you need to take screen shots to keep track of things

Simple .jpg files are enough for me to trace over or scale and pull dimensions off of.

No pattern making is as far as I'm likely to go and only then really if I'm working with someone else. For one offs Fabrication or cutting from solid is my preferred option

 

[GreenTwin]

No pattern making is as far as I'm likely to go and only then really if I'm working with someone else. For one offs Fabrication or cutting from solid is my preferred option

It is only a matter of time.
Don't try and resist it.

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[Richard Hed]

I think we have pretty much beat this horse to death.

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no NO, I saw it breathe--give it another kick!

 

[GreenTwin]

no NO, I saw it breathe--give it another kick!

I already buried it.

.

 

[petertha]

@GreenTwin actually I have done 3D modelling from imported reference pictures so I'm familiar with both the process & the issues. Mainly Rhino 3D which actually had significantly better tools than ACAD or other regular 2D apps. And mainly aircraft bodies which is swervy curvy stuff, harder to pick & compare references. SW tools in this regard are another step above. I never looked back because the power was that much better.

One of the headaches is quality of the reference itself. An old 2D drawing can have multiple levels of distortion starting from the initial ink fingered draftsman, through to paper publication, then maybe scanning. Often I'd be zooming in splitting jogged pixels occupying most of my screen. So one has to set reference geometry lines/points & work off of so called 'known' dimensions. Its always shades of compromise, what part of the drawing do you believe more than the other. I would guess you are very familiar with this judging by your work. Reference photographs are yet another can of worms. New sources of distortions; focal point, perspective, lens distortion...

I think I posted this SW link but I would encourage you to just digest the initial part of the high speed video (the rest is mainly surfacing). See how he has multiple opposing views of the model subject? If more than one view, even sectional views are available, its super helpful inside a 3D modeler like SW. Because he imports these views on the corresponding primary planes, normalizes them (by tweaking 1D stretch/shrink, aspect ratio etc) to known or defined dimensions. Then (the important bit) he draws curves & lines in one reference plane tracing a feature, then references and/or projects this curve to a corresponding other planes <ahem> entirely within SW . They are connected & make the backbone of all the features that then define surfacing operations. This workflow is best handled in a 3D app, not 2D app. To visualize a simple example think of the crest of a car fender. You can view it from the side one way & view form the top another way. But it is entirely defined by a single 3D curve that came as a result of having both views simultaneously. This kind of thing might be helpful for your future projects

http://www.solidworkstutorials.com/how-to-model-audi-r8-car-in-solidworks/

 

[GreenTwin]

Then (the important bit) he draws curves & lines in one reference plane tracing a feature, then references and/or projects this curve to a corresponding other planes <ahem> entirely within SW

It should be noted that I don't have just one way to do anything.

And my methods have been evolving over an 11 year period.

So people can be prone to cherry pick a method I was doing 5 years ago, or 5 minutes ago, and see a lot of variations, and inconsistencies, and so exclaim that this is a "gottcha" moment. Its not that simple.

I don't dwell too much on my 3D model approach, or whether I am always absolutely consistent.

It is more of a mix-and-match, make it up as you go, ............because..........well I can; its a hobby and I don't care how exact it is, nor do I really care if others approve my methods.
I just throw stuff out, and if people want to use it, more power to them.

I watched a lot of Soliworks videos in 2011, trying to learn SW, and while the models I saw with the very impressive compound surfaces were state-of-the-art design work, much of that was not easily applied to building a model engine, or overly complex for a model engine design.

I see Solidworks at a buffet, where you can walk along and pick and choose whatever you want, as little or as much as you want.
You can always go back and get more mash potatoes, but you don't have to ever eat mash potatoes.

I use SW features/functions a la carte, often only learning a feature because it does something I need done, such as creating coreboxes for molds.
I don't use sheetmetal, but SW has great sheetmetal tools.

As I mentioned, I often capture geometry from an existing SW sketch, and paste that into a new sketch, so that mating parts will always be exactly the same dimension, and have the same reference back to the origin.
I use this feature extensively, in SW.

To sum it up, there is no one-way that I do things.
If it works well and saves time, I use it.
If it is just "recommended as good practice", I often ignore it, because like I said they use to say "You MUST set the limits in your drawing" in AutoCad.
If I had a nickle for every piece of bad advise I have been given, I would be a billionaire.

You have to evaluate which features give you the best bang for the buck (time), and the features which work best for your engine design.

.

 

[Richard Hed]

All this noise about SW. Doesn't anyone have some noise about Inventor?

 

[Jasonb]

I doubt there are many hobby users that could afford either