Redraw old drawings

[EngJW]

How do other people approach a situation like this?

We have lots of old pencil drawings that are 30-40 years old or more and are converting them to cad drawings. Some guys want to just redraw them in Autocad but I am trying to do them as solid models.

Trouble is, these are complex castings and it looks to me like many of the sections were drawn with triangles and circle templates and then scaled to get a dimension. All dimensions are in fractions. If you try to reproduce these in cad you find lines that don't connect, lines not tangent to curves, and on and on. Of course, Solidworks refuses to accept anything that isn't dead on. Some things that look ok in a section view do not work out in 3d. I think the pattern makers had some liberty just to make things blend together.

My approach has been to take all the fractions and round them off to 2 place decimals. If some of the features on the drawing cannot be defined the same way in Solidworks, I try to find an alternate dimensioning method that will give just about the same result. This gives the checkers fits because they want exactly the same views and same dimensions to check off.

Some others are using 3 and 4 place decimals to design but then round off to 2 places (plus or minus .030) when dimensioning. I prefer that the design feature and the dimension be the same, and foundries don't work to 3 places anyway.

Is anyone out there faced with a similar situation, and what is your approach?

Thanks,
John Woodward

 

[SBaugh]

Try using the 2D to 3D toolbar. The list of icons there is a "repair sketch". That might help you with problem sketches. Also use Tools\Sketch tools\Check sketch for feature. This only if your converting the ACAD drawings to SW parts.

Some things that look ok in a section view do not work out in 3d.

The problem with ACAD. ACAD gave the user the ability to do what they wanted whether it was right or wrong. With SW your section views will come out like you build them. There is no way around that. If your Boss doens't like it or others, then you should explain to them that there is nothing you can do because what you did is right according to the model you built. If the model is wrong then that
s another issue, that we cannot handle here .

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.scottjbaugh.com

Merry Christmas
faq731-376
faq559-716 - SW Fora Users

 

[TheTick]

Many of us have woked at places with an archive thousands of 2D hand drawings.

I worked at a place that was 75 years old. The product line was tried-and-true, so there were many old parts still in production from hand-drawn prints.

The industry being what it was, we used many of these old parts in new designs, and found the need to model many old hand-drawn parts. Not a big problem from a modelling standpoint, but a real headache from a PDM stanpoint.

We ended up modifying the ECR process to accomodate CAD models for hand drawings. Basically, it went like this:
1.) manual drawing updated with single line note to show the part had been modelled
2.) CAD model created
3.) drawing portion of CAD model was a simple word drawing that said manual drawing was master. This was in UniGraphics, so drawings were contained in the same file as the model.

"Customer satisfaction, while theoretically possible, is neither guaranteed nor statistically likely.--E.L. Kersten

http://www.EsoxRepublic.com

 

[TheTick]

On thing I found from modelling from old and drawings was there were often "fudged" dimensions that didn't match geometry. In that case, dimensions must overrule.

Sometimes, fudged dimensions resulted in shapes that were not geometrically possible in normal time-space. Then, it was time for detective work, which often exposed an ugly web of tribal knowledge as to how the part was really supposed to be made, as oppposed to what the print said.

Not too healthy from an ISO/QS standpoint.

 

[MadMango]

2D hand-drawn conversions to 3D is always a pain- i.e fudged dimensions or poor drafting quality resulting in impossible geometry.

We had a few hundred drawings that we converted to SW drawings and models, a few hundred still to go. We approach this in two ways. 1) It is busy work for new engineering members. It allows them to get used to our network file locations, gives us an ability to see how they work, 2) If a part with a legacy drawing goes through the ECO process, it gets updated to SW.

We always build the model to the dimensions on the print. If it's fractional, we input fractions in the dimension box, if it is rounded, we leave it as such. If we come across a problem, we then reference back to the sampling inspection that QC/QA has on file for the part and adjust accordingly. If that doesn't resolve things, we grab the physical part and reverse engineer it so the model and drawing accurately reflect what we have on-hand.

[green]"But what... is it good for?"[/green]
Engineer at the Advanced Computing Systems Division of IBM, 1968, commenting on the microchip.
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[ctopher]

I redo old hand dwgs and obsolete cad dwgs in SolidWorks everytime. I can redo them faster than 2D-3D or importing DXF. The more I do, the better/faster I get with SW. I also make sure all tolerances match the original, if SW will not do it, I write an EO to make the change if possible.

 

[CorBlimeyLimey]

If the drawings are redrawn in AutoCAD they will have to draw all the views (front, top, side, etc) individually and any later mods will have to be individually reflected in each view.
If you redraw in SW, basically, only one sketch is required & multiple views (including Iso-, Tri- & Di- metric, Sections, etc) can be had at the touch of a few buttons. Also any later mods need be made only once on the model & all views will be updated automatically.
IMO it's a no-brainer choice ... if they choose the AutoCAD route, it shows they have no brain.

 

[ctopher]

CBL ,I agree.

ACAD ...
(20 years behind others IMO)

 

[drawoh]

jlwoodward,

I agree with your checkers. If you can reproduce the old drawings exactly, then you have got the geometry right.

The difference between drafting boards and slide rules, and mechanical CAD is that you cannot get things exact. Try using the correct geometry and fractional dimensions, and rounding things off. SolidWorks allows this. 1/32" is a perfectly good approximation for something like 0.031167". For that matter, .031" is a good approximation for it too.

JHG

 

[EngJW]

Drawoh,

The old drawings may not be right in many cases. Dimensions are often fudged and changes are made without correcting the drawing view. Plus, the parts are fudged compared to the drawing, or maybe the other way around.