Transformation of manual drawings to 3D CAD 5

[maxiedog]

SW novice seeks help on strategy to adopt when faced with the problem of converting legacy manual drawings of auto engine to 3D CAD. There are 40+ drawings. Initial thoughts were rasterise & then vectorise to DXF ( the only format supported ) with Scan2CAD & then import somwhow to SW. I am sure that all in the community will have faced this problem before but no results from search. Many thanks for any guidance.

 

[rockguy]

I have always found it easier to just start from scratch when converting from 2D to 3D. Sounds like you have the prints so just layout sketches based on the prints and extrude, cut, loft, revolve, etc until you have what you need. The biggest problem you will face when trying to use the 2d dxf geometry is gaps and overlaps in the lines. I find by the time I do all the work to make the dxf usable I could have just sketched it out directly in SolidWorks.

 

[ctopher]

We just transferred a couple hundred dwgs from Applicon Bravo via DXF. This is for reference and archive only. It is much faster and better over all to re-create in SW from scratch. Rockguy is correct.

 

[SBaugh]

(DXF files) Depending on their complexity I would normally re-create them but if complicated I would use the 2D to 3D tool. See the help on it, if you have more questions you should contact your VAR.

You could put images on sketches to work from (Follow) in SW, but that is the long way to build it.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[TheTick]

A major problem with the 2D-to-3D scenario is that you get what is drawn, not what is dimensioned. This problem could be even worse for paper drawing conversion, where it is likely that changes may be made by simply changing the text of a dimension without changing lines.

Accuracy of a paper drawing is limited to the fineness of the pencil line. The maximum accuracy for this would be about ±.01 inch under the absolute best circumstances (good drafter, clean paper, sharp pencil, etc.).

There are many people out there stumping for 2D to 3D redraw work. If you can't spend too much company time on the conversion, outsourcing should not be too difficult or expensive.

If the ladies don't find you handsome, they should at least find you handy.

 

[Theophilus]

Normally I start from scratch as well. In doing so, I sometimes come across errors in the existing prints that require the discovery of the true design intent to correct--so this can be a good practice merely for that reason.

Other methods of importing (sometimes even from CAD drawings) are even more tedious than starting from scratch. After doing a part or two, you will probably find efficient methods of modeling the parts in 3D yourself. It's a great way to practice good design while using SolidWorks (considering future editability, assembly placement, etc.). Even with Rhino 3D parts I have found starting from scratch the quickest method.




Jeff Mowry
Industrial Designhaus, LLC

http://www.industrialdesignhaus.com

 

[maxiedog]

The consensus seems to be to redraw from scratch to get the benefits as stated or outsource. Thanks to all respondents. I think you probably saved me a lot of frustration.

 

[JNR]

I agree with all the comments made. Plus you have additional issues when trying to input from hardcopy. Manual drawings are not accurate enough for CAD system use to start with. (Can you draw accurately to 8 decimal places? I think not.) NEVER fake dimensions on a CAD drawing. Then when you try to scan, all kinds of problems come up. First, the paper has stretched or shrunk and not even uniformally. Then you can't get the paper perfectly aligned. Then all you get a raster picture of a piece of paper which has no real accuracy. And that's before you spend time on all the vector/DXF/2D-3D stuff, etc. It is more trouble than it is worth and in the end it will come back and bite you in the @$$ when you least expect it at some time in the future.

Here is something else we have discoverd. Those drawings might not be quite a perfect as you think in describing what was intended by the designer. However what you have been manufacturing for some time (and presumably works fine) is what the drawings actually show. If you model manually by reading the drawing and recreating the models, you will make nice new models in your new SW (or other CAD system - same principle) of what you have actually been manufacturing. That is a very good thing. We found this out by accident the hard way. We never try to bring over 3D data in any form from our legacy (wireframe/surface) system (appart from the fact that IGES is worthless.) We always model from scratch. In the end it is quicker, easier and heads off future headaches.

3/4 of all the Spam produced goes to Hawaii - shame that's not true of SPAM also.......

 

[TheTick]

So now what?

SolidWorks has a few tools to help the 2D to 3D transformation.

The 2D to 3D toolbar is likely to be of little use in this case, since you only have scanned images to work from. Still, it is a tool set worth getting to know.

Of more value in this case is SW's ability to bring in bitmap and tiff files. These will allow you to overlay SW geometry on top of scanned images.

There are two ways SW can use images. One is using TIFF images as a background. This isn't really that useful here.

The other method is to insert a bitmap version of the scanned image into a sketch, where it can be moved and scaled. You could insert the same drawing image multiple times on different planes, line up the different views to your liking, and sketch away. See the help files under the "bitmaps --> in sketches" topic for details.

If the ladies don't find you handsome, they should at least find you handy.

 

[Cryo1]

We have a couple HUNDRED drawings to update from the 1960's to present. When we need a new revision, we produce the 3D model then the drawing. When we need the part in a 3D assembly, we produce the assembly then go back and make a drawing file when we need it.

It will take us about 2 years at this rate to convert our old blueprints to slddrw formats.

We are finding a ton of problems with the old drawings. Doing pencil and ink in the past was very time consuming so I'm not to harsh on the old work. Of course, if the drawing has been around for 30 years but it was incorrect, did it matter? Some human corrected or compenstated for the mistake along the way but that doesn't allow for incorrect drawing files.

 

[JNR]

Sounds like Cryo1 is doing exactly what we are - building the models and THEN making drawings from them AS THEY ARE NEEDED. It seems like a pain and you should see the program managers bitch about the hours when it affects one of their projects. In fact it does not cost any more than if you were designing new parts from scratch which is a little consolation. BUT it pays dividends in the end and you don't create a bunch of unforseen problems done the road. Also sounds like Cryo1 has found out the same thing I spoke of. The drawings (even legacy CAD) were not all perfect, but someone interpreted and you had good products. If you are now putting them into modern accurate solid models, might as well - no, you NEED to - build models of what you are actually manufacturing as interpreted from the old drawings.

I would also make the following comments. There are two basic things going on in this thread and they are separate issues with separate problems. One is 2D to 3D assuming you have accurate data initially. The other is inaccurate scanning of questionable accuracy data into 2D in the first place. Frankly the amount of effort involved in the latter and the amount of potential future problems makes it a dead issue as far as I am concerned. Further, I submit that the time required to build a model from scratch by reading a drawing (and getting good design intent into the model!!!) is little different from taking 2D views and "building" a 3D model from it by semi automated methods. That stuff was only included in the first place as a sales tool - a crutch for those who were a bit afraid of launching into the 3D world and mostly aimed at entrenched 2D AutoCAD users. (That's not intended to be a criticism of any kind - as an ex CAD VAR I have been there, seen that many times and years ago too.)


Be naughty - save Santa a trip.

 

[ShaggyPE]

Well put JNR, I agree whole-heartedly.

 

[mushin]

This may be of little use to you, but I will suggest it anyway. About a year ago I bought 5 copies of TurboCAD 5 at the local software liquidator, to give to my clients for the purposes of having an inexpensive AutoCAD type system. This way, they could print and manipulate my SolidWorks generated, but saved as AutoCAD, drawing files. At 15 dollars a copy it was a bargain! In fact, it is better software than AutoCAD LT.

Anyway, TurboCAD 5 has the ability to turn scanned files into DWG format. It will run on any old 486 computer, freeing up the decent machines for your day to day stuff. From there you could manipulate the files in AutoCAD or TurboCAD to give you the 2D sizes that you want. Then you could import it into SolidWorks for the 2D to 3D translation.

Hope that this may help...

Jim Barron, C.E.T.
Update Design Services,
Mississauga, Ontario,
Canada
JamesFBarron@aol.com

 

[JNR]

Hmmm......... have we been listening to what we are reading, people? If all you want is preserve printable copies of old drawings, then put them in Adobe pdf's. Then anyone with a computer will be able to print them forever. If you want real 3D models with anything like accuracy FORGET SCANNING!!!!!! This is of course an oxymoron, because if you are making solid models, you NEED PERFECT ACCURACY. If not it is going to come back and bite you in the @$$ VERY VERY HARD one day soon. That is expensive - much more so than doing it right in the first place. If you can't afford to do it right you are either underfunded, in the wrong business, or serioulsy and unrealistically under bidding your work.

Here are a FEW of the horrors of scanning.

1. Paper, even mylar suffers from non-uniform expansion and shrinkage with temperature, humidity, age, physical handling, etc.

2. Plotters do not give you perfectly accurate plots in the first place - certainly not accurate enough to create solid models from.

3. I defy you to get the scan perfectly square to the plot - even with the magic software. C'mon, the original isn't that straight anyway.

4. Scanning is raster for crying out loud. Is goes in finite incremental x/y steps!!!

5. Line weight/quality - where is the true center (and ends) of that line?

6. Do I need to list more..........?

Now, sure you might find an "apparently acceptable" work around for some of these things (remember to wear your kevlar underwear, though) but you are never going beat them all and you are going to invest large amounts of very frustrating time and money in trying.

Rebuild the models manually (and thus from them the drawings if necessary) on an as-needed basis.

Be naughty - save Santa a trip.

 

[Tmoose]

RE:drawing to scale, and accurately.

We had a 1000 lb casting machined.
The CNC machine tool could import geometry directly from dwg format info.
In a drawing derived from SW 2001 we had apparently cheated on a dimension. The bolt pattern was made on the "drawn" diameter not the "dimensioned" diameter. Big mess. Lots of delays finding the problem, the cause of the problem, and then how to salvage the part.

The contact I have had afterwards with a few (other) machine shops suggests they do not usually import geometry directly, with no explanation as to why. I guess I'm glad to hear that, although I wonder how tolerances can be "programmed" in, unless the thought (hope) is to simply aim at the center, and figure the CNC is "better."

 

[JNR]

You don't program tolerances per-se. You program the NC machine to hit the right spot. Tolerances are there on the drawing because there is variance in the process. Tool wear, machine tolerances and wear, temperature, etc. etc. However if you include tighter tolerances than you need on many of your dimensions, all it will do is tend increase the cost of your parts because the machine shop has to figure in to the price the scrap, rework, additional manual care of tooling involved in meeting them.

One of the reasons some machine shops do not use the electronic data given to them is this - some people try to second guess them and bias their tolerance. So the actual model dimensions are not the nominal design dims and they can just use them for NC programming and expect to make good parts.

John Richards Sr. Mech. Engr.
Rockwell Collins Flight Dynamics

A hobbit's lifestyle sounds rather pleasant...... it's the hairy feet that turn me off.

 

[Amear]

As to previous posts, I was wondering if anyone has found a program that will convert 2D Bravo files to SW or pdf in mass amounts. (for presorvation purposes) Our company is going through a retrofit in joining with another company and we are responsible to transfer our 20 000 drawings from the past 15 years. Price of program is not something we are too worried about. Thanks for any help.

 

[ctopher]

We have thousands of Bravo dwgs. We were unable to convert into SW as you state. As dwgs update, they are either redrawn created as models in SW, or DXF. We had someone sit down and go thru each dwg and convert to DXF, then archive Bravo.

 

[TZellers]

Been there done that. Scan and pdf for file keeping. Start from scratch for 3D models.

I've found the SW toolset is pretty good as The Tick points out. Inventor (V6) did not have the bitmap feature. Also, SW allows you to print your sketches at scale, so you could print and compare to the original drawing. This was a big deal when trying to replicate impeller drawings from the 1950's. You wanna talk about pencil thickness and dimensions......

The other thing to do is engineering archeaology. If you have the original vellum papers, you could hold them up to the light and see where the holes are (for curves), etc. Usually, most people design to 1/16 or 1/8 or something consistent. You can kinda determine the intent of the drawing and go from there.

 

[StiLLiving]

Scanning, rastering - vectorizing - would be a long way to go. Even though there is a helpful tool in SW to do it (see TheTick's post above).
Build 3D model usind blueprints as a reference, generate 2D prints and save them in either format - this is shortcut and the only way to store an accurate and precise
CAD data.
I'm positive on this.

Regards,
G.