AutoCAD users to Solidworks 1

[seghojangan]

Dear all,

I am sorry that maybe this is an ordinary question, but I post this on Solidworks forum and a local forum and still no respons. I've been searching the whole week regarding this question on youtube tutorial but stiil no luck - or maybe I still could not find the right directions.

So forgive me if I have to asked this.

I am a autocad user and willing to move to Solidworks or if I still could not get the answers I will try Inventor.

At some online tutorial, also on Youtube, always explained that to works with Solidworks is always starting with creating parts.

But in what I always do in my job as Furniture designer I always starting with sketch - full 2D drawings - 3D and then parts components.

as image below:

Is Solidworks could do the same way? or there is a similar way?

If so please point me to the correct directions and if possible a tutorial.

Thank you in advanced.

 

[MadMango]

To be clear, you create the hand sketch, then make the 2D drawings, then build the 3D models in AutoCAD? If so, your workflow will have to change a bit when using SolidWorks. You can still use your hand sketches in SolidWorks, then bring them into SolidWorks to make the 3D models, from those the 2D drawings are made. Look for any tutorial on YoutTube for surfacing, which usually starts with bringing in a concept sketch to base the models from.

"Art without engineering is dreaming; Engineering without art is calculating."

Have you read faq731-376 to make the best use of these Forums?

 

[seghojangan]

Hi MadMango,

Thank you for your response.

Ok I will have a look on youtube. I will comeback here if there is more questions.

 

[TheTick]

The short answer is that nearly any 3D CAD can do what you want, including SW.

Most of my work is done with master sketches used to create parts. Two or three sketches in an assembly control geometry in a multiplicity if parts.

 

[seghojangan]

Hi TheTick,

I am sorry but I could not understand your explanation.

You mean, for example, I can create a full Table assembly in a single window?

Would you please point me a correct direction how suppose I do that?

As far as I know, in Solidworks we create part per part first and then assemble it together.

If I can bring my 2D sketch (I mean a full drawing sketch, not component sketch) from autocad to Solidworks and then I can create parts component based on my 2D drawing, it would be helpful.

Please, give more clues about it.

Thank you.

 

[MikeHalloran]

Solidworks allows something called 'In Context Modeling', I think, which is sort of like starting with a skeletal assembly model, and building all the component parts within it, while still keeping the component parts' models as separate files.
I managed to get myself pretty confused with it, but I got less awful after a while.


SW also has a 2D to 3D conversion facility, which allows you to paste orthogonal views to orthogonal planes and to construct 3D models from those views. No, it's not automatic, and there's a learning curve (beyond that for just grokking SW), but it works.



Mike Halloran
Pembroke Pines, FL, USA

 

[seghojangan]

Hi MikeHalloran,

Thank you. Looks like I got some enlightenment from your reply.

I am in process watching the assembly models tutorial in youtube.

http://www.youtube.com/watch?v=tWvRa5-rWuQ[/URL]]

Hope I am in the right direction.

 

[Jboggs]

You need to research a topic called "top-down design". Think of component parts at the bottom of a pyramid with the final assembly at the top. Bottom up design starts at the bottom (component parts) and proceeds to the top (the final assembly). Top-down design procedures allow you to start with the concept at the assembly level and create individual compontnents based on that concept.

 

[EEnd]

In addition to "in context modeling" and "top-down design" suggested above, "layout sketch" and "assembly skeleton" should be useful search terms for finding tutorials on how to accomplish what you are after.

Eric

 

[mjcole]

2d -> 3d and Layout sketches are both great ways of doing what you want. Thank you for the attached pic, I'll try to do an example of another part only or (Multi Body) technique that uses 2d & or 3d sketches to achieve what you want. Another functionality you may find useful in the Future. See the help tutorials for more info.

"It's not the size of the Forum that matters, It's the Quality of the Posts"

Michael Cole
Boston, MA
CSWP, CSWI, CSWTS
Follow me on !w¡#$%
@ TrajPar - @ mcSldWrx2008
= ProE = SolidWorks

 

[SBaugh]

You can import 2D drawings into 3D Parts, you will have some to clean up and repair all the imported sketches, because the importing and because of AutoCAD usually causes double sketch lines and SW won't extrude sketches with double sketch lines.

You can use the 2D to 3D toolbar to fix the sketches and repair them. You can also try using Sketch Contours to create your design from a single sketch. I am not big fan of this style of designing, but it does work.

IMO if you have the dimensions it would be quicker to just make it all new in SW, part by part or body by body (in a single part).

I have to deal with AutoCAD users all the time making their way over to Solidworks. Its much harder for them than it is for others. First thing you have to do is stop thinking like AutoCAD and stop trying to make Solidworks act like AutoCAD, because it doesn't. There are a few things to help out, but eventually if you stay with Solidworks you will learn to like the software and understand the principal behind it. All of ACAD users that have switched here never go back to AutoCAD.

Regards,

Scott Baugh, CSWP
Berry Plastics
Cad Admin\Design Engineer
GEASWUG Greater Evansville Area SWUG Leader

http://www.scottjbaugh.com

"If it's not broke, Don't fix it!"

faq731-376

 

[MikeHalloran]

I am one of those crusty old AutoCAD users of whom Scott speaks.

In a couple of years of OJT and banging on it, I came to love Solidworks for the speed with which I could generate a decent 3D model of most anything I could measure or imagine.
... and to hate it for its sometimes bizarre internal logic,
for phase errors between the program and the help files,
and mostly for my inability to make it produce a decent looking drawing in _my_ style.

In fairness, the only training I got was a few minutes of lightning quick 'new school/ old school' demos by an experienced user who soon left, and a couple of free seminars by the VAR, who really did add value.
The help file exercises really were helpful, but the user interface had changed _a_lot_ between the version I was using, 2008..2010, and the version the help files had been produced with, 2006..2007. I _hope_ that the help files have by now been updated some.
I did not have access to the tutorials on YouTube, because YouTube was completely blocked by our IT department, they would not make an exception for me, and my home computer couldn't run SW.
That job disappeared in 2010.

Now, I've got half an offer, sort of, from a guy who wants me to work irregularly, part time, but he wants me to work at home and use my own computer, and he clearly doesn't want to pay a decent rate. To run SW, I'd have to buy a new computer, which is sort of okay with SWMBO, and provide my own copy of Solidworks, which was not okay with SWMBO when she found out what it costs, and which I can't really justify for work that may or may not materialize.

Meanwhile, for my own projects, I'm using Draftsight, a 2D AutoCAD clone, and wishing there was an open source version of Solidworks, because working with AutoCAD or similar is not nearly as much fun as it used to be.


Mike Halloran
Pembroke Pines, FL, USA

 

[seghojangan]

Dear Jboggs, EEnd and mjcole,

Thank for input and support. I am still in progress trying to jump to Solidworks.


hi SBaugh,

Thank you for your input.

I am also using Sketchup to support my works so far since is simple and also fast to translate my paper into virtual Data.

yes it has been told to me that we have to change our thinking from AutoCAD if we want to jump to Solidworks. And I am ready for it.

What I am looking for is it Solidworks could accomodate my working system? Everytime I search tutorial from the internet it's always explained that working from Solidworks is start from Parts. But what I usually do is to build something is starting from full design concept and end up with Parts as my 1st post above.

If Solidworks can import from Autocad, it would be very helpful but if not I can still try to draw from scratch in Solidworks.

Of course I am willing to learn and use Solidworks and now I have try to use it and looks promising with constraint and the concept, but for me it's not really help yet before I find a way to use it as what my working system do.

 

[SBaugh]

Well you can build all your parts as bodies inside a part and use the Insert\Save Bodies command to take all the bodies and make them into parts and create an assembly at the same time. However the one big problem I have with this command, is if you rename something or move its location, or delete the original part you made the parts you created cannot get the link back and the file will be permanently broken. The other big problem I have with this commend is you lose the part features from within the part. Meaning you can only change it at the original creation point. I personally don't recommend building it like this, because its very easy to break a link and when that happens you will not be able to go back fix the link, which will cause you more time and money.

I think building the parts and working your way up is the better solution, even if its top-down. They don't have to be perfect, just close then you can adjust them in the assembly. You can even edit the parts in the assembly and modify them. I made an example for a friend in our User Group here. They make furniture and he was looking for a more efficient and faster way to create their models. I made a Top-Down (incontexted) assembly Model from the parts he gave me. Now its easy to change 3-5 dimensions and get a completely different model and design.

Scott Baugh, CSWP
Berry Plastics
Cad Admin\Design Engineer
GEASWUG Greater Evansville Area SWUG Leader

http://www.scottjbaugh.com

"If it's not broke, Don't fix it!"

faq731-376

 

[seghojangan]

Hi Scott,

With starting to make parts first in Solidworks as your suggestion, it is mean I have to make the design first on other program for example Autocad and then import it to Solidworks as parts based or could I make the sketch / idea design in directly in the Solidworks?

Please point to the simple tutorial regarding this, because if creating parts is the best way to enter the Solidworks, in my opinions, solving this problems would be the main key.


Michael Cole,

Would you please advise which help tutorial would guide to solve my problems?

Also I am looking forward for you example.


Thank you all in advanced..

 

[MikeHalloran]

Sketching and then adding constraints or dimensions in SW is >>>WAY<<< easier than drawing 2D or constructing 3D in AutoCAD.

Importing stuff from other packages is nice if you have existing designs, but don't even think about doing it for new designs.



Mike Halloran
Pembroke Pines, FL, USA

 

[SBaugh]

Honestly... since your new to the software go through the Help online tutorials its the best and fastest way to start. I recommend this method to all users. Once your done with that I would recommend getting Essential training from your VAR. This will give you a much better understanding of essentials in Solidworks.

I took your image above and just made a quick example of it. I don't have any dimensions to work with so I guessed at it. Now that I have a few parts I can make it look however I want to by changing the dimensions, especially if have the basic profile of each part. if the profile is wrong I can always go changes it... but not knowing the dimensions is OK in SW, you don't have to know everything, just the basics and once you get that down and look you want, then you can worry about the details. Its how we do all our Plastic designs. We try to keep it basic, but we don't worry about the volume until we get the look we are after. I try to keep it close, but until I have a design in mind, I won't know what the volume is going to be right away.

I was going to post an image, but our IMS team has blocked the ability to upload images recently, but I was able to attach the files. They are 2013 files.

Hope these helps you understand, you don't have to have a finished or completed project when you are using SW, just need an idea is all. If you do have a completed job, that just makes it easier to create each part.

Kind Regards,



Scott Baugh, CSWP
Berry Plastics
Cad Admin\Design Engineer
GEASWUG Greater Evansville Area SWUG Leader

http://www.scottjbaugh.com

"If it's not broke, Don't fix it!"

faq731-376

 

[richardfoodindustrie]

Hi seghojangan

I did reply to your post at the Solidworks newsgroup but it got
removed by Solidworks because I mentioned to look at Autodesk
inventor and fusion and posted a videolink.

Here it is again.

https://www.youtube.com/watch?v=pMcsQjxDSH8

I don't like to type it all over again but
you could look at a good direct modeler. It has more flexability
and they have improved the last years.
You could look at Spaceclaim, Autodesk Fusion 360 etc.
We have been using Solidworks for 19 years and before that we
used Autocad 2D. We want to have direct modeling for our
conceptual machinedesign because it is much faster and have run
out of patience with Solidworks. They anounced it 4 years ago and till
now it still doesn't exist. We are also experience quite some bugs that
take too long too fix. There are major problems on high resolution
monitors with the latest releases, you can't even see your
dimensiontext in the edit dimension menu if Windows scaling >150%.
Althoug I got an SPR number one year ago they still didn't fix anything.
They even think it is fixed while it has gotten worse.

https://forum.solidworks.com/message/401519#401519

Solidworks is not the company that I know from 10 years ago, it is
now really Dassault, they invest in "3D Experience" and I am afraid
that CAD development suffers from that.

 

[snowshoe2]

Hello Seghojangan,
In many ways It doesn't matter which 3D tool you choose, the skills you learn are transferable (a good portion anyway) I have used 3 different ones and found a way to make each be productive. I currently use SolidWorks and have in a few different industries (each requiring different methods). I look at the competition just to keep current of the other tools and haven't seen enough to want me to change away from SolidWorks.

I agree with Scott Baugh, zip thru the tutorials, go to training if you can and find a user group to attend for more development and help. I have worked with many people going from Acad to SW and found once they understand the basics of parts, assemblies and drawings they can build almost anything they need to. It just takes a bit of time to develop a new skill set. Even pay for a tech dude from the VAR to spend a couple of hours with you to get you going in the right direction with your own products.

Have fun
Steve

 

[SBaugh]

Per Richards post on direct modeling... SW did release "Mechanical Conceptual", which is part of Dassualt

http://blogs.solidworks.com/solidworksblog/2013/01/introducing-solid.html

but is also part of Solidworks as well. I have been using SW since its release in 1995 and believe me SW has changed dramatically in its first 5 years of its life... there is a good reason its not the same product it was 10 years, 15 years ago +. If it was it would be like AutoCAD's 2D software and never change. Solidworks and Dassualt is not making the same mistakes Autodesk did. They are changing with the times, I think the real problem for you and I Richard and most other veteran users, is we are not changing as fast, at least I am not. I am trying to keep up, but it changes so often. I think Change is good in software, means we are getting more options, some might be in their infancy stages and might be buggy, but I am sure in time they will work out.

As for SPR's unless you get more people to agree and turn in your bug\SPR# it will never get repaired. I suggested that SW have Part and Assembly Statistics... to help find slow features or mates, etc... Though a good idea at the time 1996-97 we didn't see it until some time in the late 2000... Though that was an Enhancement SPR, its the same for bug reports, especially if its not keeping you from doing your work and you have a workaround, no matter how cumbersome.

Enough of hijacking this thread... back to the subject matter:

seghojangan - I hope the attached models above helped you understand the basic of how easy it is to just create parts and place them into an assembly and if you have to place some detail in the parts for assembly. Though the parts in the assembly are not right, its easy to change the parts in the assembly and not worry about clicking back and forth. - Let me know if you need further help with this.

Cheers,

Scott Baugh, CSWP
Berry Plastics
Cad Admin\Design Engineer
GEASWUG Greater Evansville Area SWUG Leader

http://www.scottjbaugh.com

"If it's not broke, Don't fix it!"

faq731-376