WhatÆs the quickest way to make dimensioned machining drawings? 2

[aliensquale]

I have a machining company and we for years have been using 2d cad systems such as AutoCAD, GeneralCAD, etc. Now we are starting to adopt 3d because everybody says it's so much more powerful, etc. I agree it's nice to have a model that you can see and manipulate onscreen... but I see that it almost creates double the work to make the model, then go ahead and create a 2d drawing out of the model, dimension the drawing appropriately, print it out and give it to the machinist to make. It's like doing work twice for one part. You first have to make a model, then make a drawing and dimension the drawing. The import dimensions feature in drawings is terrible, it never puts the right dimensions in the right places, etc. so you manually have to go and insert the right dimensions in the right places.

I know you can feed a solid model through CAM software to program your machine tools but we don't do this. We just machine parts off of 2d drawings.

so my question is, is there a way to make solidworks drawings with an assosiated model just as fast as making a standalone 2d drawing only like we used to do in AutoCAD, etc.? I don't want to significantly slow down my business and spend all day making models then drawings.. I don't have that time or resources available.

 

[Eltron]

A lot of the double work can be avoided by proper modeling practice. If you organize your dimensions on screen in your sketches and add tolerances while sketching you can do an Insert/ Model Items in your drawing. This will eliminate much of the duplicate work. Once your guys get good at using the software, they should be faster using the parametric 3D system than the old 2D system. If not, some training may be in order. Plus, with 3D all of your models will be ready for CAM and they are parametric so models will change with design changes. It may not seem like it now, but the initial growing pains will get better.

Dan

http://www.eltronresearch.com

 

[GregLocock]

Surely that depends on the complexity of the part, to some extent? I can imagine that if your lot in life is making pins and sockets, then 3D looks like an overhead that has little upside, whereas if you are making injection moulded 3 dimensional jigsaw puzzles then it pays for itself immediately.



Cheers

Greg Locock

SIGlease see FAQ731-376 for tips on how to make the best use of Eng-Tips.

 

[CorBlimeyLimey]

aliensquale,

Try creating the model as you would create it in your shop. Start with a lump of 'material' and cut away the unwanted stuff. While doing that, dimension your sketches the way you would like/need to see them on the drawing. The Import > Items function should then work much better for you.

Producing only one or two simple views in AutoCAD could be quicker than using SW, but the more views needed in the drawing the less productive AutoCAD becomes, especially when dealing with sections, details, etc.

 

[Tobin1]

Howdy,

CBL's suggestion "model as you would create it in your shop" is a real good practice on many levels. Although in some cases that can be difficult.
Depending on your particular situation/need it might be possible to eliminate the "paper" drawings. If the machinist can view the model with the dimensions it may not be necessary to make a paper drawing. You wouldn't be the first to do this. Some think this is the future of drawing/drafting.

Just a thought




Tobin Sparks

http://www.nov.com

 

[ajack1]

aliensquale, I do not wish to sound rude but you seem to have chosen 3D for the wrong reasons.

As others have said with good modelling practices and experience things will get quicker and easier and it is my belief that almost anything can be modelled as quickly and produce drawings as quickly in 3D as in 2D, but that does cost time and money and for very little gain.

Basically a pencil and paper drawing allows you to program a machine, 2D data lets you use CAD to pick points for drilling etc and use profiles for 2 1/2 machining 3D models allow you to machine directly from a model and are the only way to go if the parts cannot be defined in 2D or involve lots of complicated sections and views.

It does not sound like you want or need 3D so why use it?

 

[rollupswx]

I worked for 8 years out on the shop floor running all of the manual and CNC machine tools. I also taught manual machining and CNC programing for 5 years.

At first making the transition from 2D to 3D might seem like double work. But as stated, unless you make the most simple of geometry 3D modeling will pay off in the long run with fewer mistakes, and indeed faster 2D drawing creation. But it doesn't happen overnight. Probably takes 6 months on simple stuff to break even on time. For more complex features, assemblies and especially moving mechanisms 3D can pay for itself on the first job.

I have found that some people cannot make the transistion from 2D design to 3D modeling. I would argue, base on my experience, that they actually weren't very good at 2D either. They depend on the experience out on the shop floor to cover where they lacked in 2D design ability.

Training is critically important. Learning how to use a 3D modeling program is a professional endeavor and deserves professional preparation.

Your designers should take to 3D design like a duck to water. But it does take 6 months or so to really start to get efficient and for the next 2 or 3 years after that the really power user stuff is brought into the picture. Even after a couple of years experience your designers will look back at stuff they did in any previous 6 months and shudder when they realized how little they knew.

 

[handleman]

SolidWorks/3D CAD is not really a drawing creation tool. It is a design tool. If all you are doing is creating paper drawings of existing parts for your machinists then perhaps SolidWorks isn't really right for you. You can chuck up a phillips bit into a 1/2" hammer drill and hang drywall with it, but you'll get awful tired after a couple of hours.

-handleman, CSWP (The new, easy test)

 

[aliensquale]

Thanks to all that replied, this indeed seems like a very helpful forum (probably the best Solidworks forum online) and I'm very glad I have found it!

Okay so basically let me give you all some examples of parts I make. This will help to better understand the complexity of the parts (or non-complexity that is) which we machine. Take a look here:

http://www.thewholepkg.com/images/Photo_Albums/Change_Parts/index.html

Basically most all of my parts can be made on CNC lathes and 3-axis CNC mills. I do some little 4-th axis rotary table milling as well but not much. I rarely do complex assemblies so I don't often need to do simulation, failure analysis, etc.

What I am finding thus far is that it really all comes down to HOW I make the models. Learning when to use a revolve versus an extrude, etc. things like that. Also, I like the idea of the previous poster to model as if it's actually a chunck of material infront of me that I am machining. I am trying to get good with using refernce geometry, such as planes, point, centerlines, etc. so I can acurately set up for instance an extruded cut on the proper plane. I am trying to stay in the mindset of, well this is how I would need to machine it, so let me try to draw it this way and use extruded, revolved cuts when posible.

I agree most of my parts are really probaby too simple to justify the switch to 3d versus 2d. But what I am finding more and more is that my 2d drawings take more time for people to understand and visualize the actual part. What I love with 3d thus far is that I can actually see the part onscreen, rotate it, cut it apart, etc. This really helps to understand all the details of the part. As a job shop we make THOUSANDS of different custom parts changing things up all the time so it really helps to have a 3d model to look at and say "oh yeah I remember that part".

Where I have just felt let down by the software is in the drawing department with dimensions. A big selling point to me was the fact that I can take my model create views from it in a 2d drawing (which works great) but then automatically insert all the dimensions into the views and the dimensions would be placed where they need to be and where it's good for my machinists. It doesn't do much good to have a dimension imported automatically into the drawing and then look at what or where it is dimensioned and say "I can't set my machine up to measure that dimension in that way!!!" So I find myself not even using the import dimension feature and instead just create my views and manually dimension the views the way I need them to be for machining using the 'smart dimension' tool. This is where it starts to feel like double work for me.

Then often times I find that some work I need to give to another shop when we get too busy and for these times I need to save my solidworks drawing as a .dxf file again putting the dimensions in where the machinist needs them. Now other shops can open the DXF file and pull any dimensions they want (based off my views I created), but wouldn't it be nice if they were able to create MORE views such as section, detail, front, back, etc. if they needed too. Once the file is in .dxf format you are stuck with the views you created originally in soldiworks.

 

[CorBlimeyLimey]

Have you discovered eDrawings yet? It is an excellent tool for allowing others to look at the drawings as well as the solid model, pick apart an assy, make measurements and even output to STL format ... and all without needing the actual models.

A self-executable can also be created from SW which allows others to view eDrawings without even having the program installed.

 

[DesignerGuy16]

It looks like there are a lot of similarities to the parts you make. Using SW to create templates of those parts with already detailed drawings will actually save you a ton of time if you're using consistent tolerancing, etc.

Even if it is different and you're using different configurations you'll find in the long run once you get used to this type of design you'll save a ton of time. We make modified atmosphere packaging machines here, and the tooling used to take 1.5-2 weeks to design, and the documentation was basically hacked together by exporting to autocad (this was in solidworks). Just bad practices. After the growing pains of modeling templates 100% and details 100% for the templates it can take as little as 1 day to design and detail a new tool from scratch.

Pay it forward if you will. Learn the program, learn it's capabilities, and then step back and think of how those will help you. Then implement it over time. You'll never get everything from the start, so just be smart about using templates, reference folder locations, etc. They seem simple, but they aren't, and implemented incorrectly will cause much more hassle then doing it right the first time.

James Spisich
Design Engineer, CSWP

 

[aliensquale]

CBL, yes I have used eDrawings, great tool, BUT I have found that if you send an eDrawing over to somebody and they open up the eDrawing file of a 2d drawing and print it, it doesn't print to the same exact scale as from printing out of Solidworks directly. For instance, my drawings are usually 1:1 scale, but when I send the drawing through eDrawings and you print it, the scale actually gets a tiny bit smaller such as like 1 : 1.15

I don't know why it does this, maybe so eDrawings can protect the authors content from printing exactly right?

-----------

James,
I looked into the templates and using configurations for similar parts. Problem is, the parts even though they look similar are constantly changing. One part may have the same O.D. but the I.D. geometry may be completely different. So if I already have a fully detailed drawing template and the part I.D. changes, it actually takes me more time to go back into the drawing, create NEW views, moves stuff around, delete dimensions that don't make sense, re-add new dimensions, etc. I found it faster to just create a new 2d drawing. Now if my part was very complex or an assembly, then yes I see that a detailed drawing template may save me a lot of time. But for me this just isn't the best option.
As for using configurations in my models, again, this is good for SOMETIMES, but the vast majority of times my geometry is changing on similar parts so I found maintaining configurations is actually harder and requires more time than just creating a new model again.

Being the job shop we are, we are LUCKY if we have a handful of parts that we make the same exact way each time. All of our parts are custom made to fit into a larger machine to hold different sized items, etc. So basically the part is different just about everytime we make it. Our machinists just basically use one standard drawing of the part and they know what dimensions to change each time they need to make the part over again to fit the new needs of the customer. Otherwise we would have THOUSANDS of drawings and it would become impossible to maintain them all being that we are only a small company with liimited resources.

 

[CorBlimeyLimey]

Why would the printed drawing scale matter? It's the printed dimensions that count. I hope no-one is creating your production items using physical measurements from a drawing.

 

[aliensquale]

they don't matter in that sense, they matter because some of the parts the machinists actually hold up to the drawing to get an idea of if it's dimesioned correctly. For instance, we often duplicate actual parts that are sent to us, so our engineer draws the part up, pritns out a drawing, but then the machinist likes to hold the physical part up to the scale 1:1 drawing to make sure everything LOOKS okay before he start cutting the metal.

I have found that .dxf files print out correct scale, eDrawings don't.

 

[MadMango]

Who else at your place is working with SolidWorks? Has someone received actual training from your VAR? I am concerned from some of what I am reading here.

Our machinists just basically use one standard drawing of the part and they know what dimensions to change each time they need to make the part over again to fit the new needs of the customer.

How do they know, by what process?

Learn the program, learn it's capabilities, and then step back and think of how those will help you. Then implement it over time. You'll never get everything from the start, so just be smart about using templates, reference folder locations, etc. They seem simple, but they aren't, and implemented incorrectly will cause much more hassle then doing it right the first time.

I agree with these statements 100%, and it is the reason I am concerned for your company. SW is a great tool, but it needs to be applied correctly, in all regards. If it isn't, you'll grow to hate it and distrust all other similar ventures.

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

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

 

[DesignerGuy16]

If you're dealing with a "specific" shape, having a template of that basic thing will save you time. If you have different geometry, add a revolved cut feature. Then you only have to add 1 dimension, vs all. Even though they're different, find out what is always the same, or that you add a lot of. You can suppress/drive these specific features in tables. Or just copy the template & drawing and use SW explorer to rename & break link to template. Even if the dimensions change, it will save more time to have all of the features there ala carte than recreating them every time. Even if all you're doing is suppressing the features you do not need. Think on it.

James Spisich
Design Engineer, CSWP

 

[aliensquale]

true, what I always run into is that I have a few different parts that I make over and over, but some dimensions change each time. So what I do is copy the solid part file, copy the drawing and put them both in a new directly, go into windows explorer, rename both of them. Problem is, when I open th drawing it is still referencing the old name of the part file. So I have to copy the old part file into the new directly, let the drawing find it, then close the drawing, delete the old part file, reopen the drawing and then it will ask me to find the new part file and I choose the new one in the proper directly. I wish I knew of an easier way to copy drawings and break references easier or just change references.

 

[CorBlimeyLimey]

Use SolidWorks Explorer

 

[ShaggyPE]

aliensquale,
like CorBlimeyLimey said, use SolidWorks Explorer. There are also a couple other techniques to copy drawings and parts that will all be easier than the method you are using. Like the others have stated, you should be able to use an existing part and drawing save it as a new part, make a couple changes to the model (be it dimensional changes or adding features). When you go to the drawing, the dimensional changes will update without a hitch and you will have to do minimal manual stuff to detail the new features.



-Dustin
Professional Engineer
Certified SolidWorks Professional
Certified COSMOSWorks Designer Specialist
Certified SolidWorks Advanced Sheet Metal Specialist

 

[Russell67]

Solidworks explorer sucks (pardon my french).

Copying the part (only parts not assemblies) and the drawing to different directory is a good way to duplicate something quickly. The method you are using via windows explorer and renaming will work, however you are missing a critical step.

When you go to open the drawing we all like to double click the drawing object open, however if you single click the drawing you will see a box labeled "References" click on that and it will show you the current path of the part contained in that drawing and the new path. Odds are they are the same.

Now double click the one on the left and navigate to the renamed part.

Close that dialog box and complete opening up the renamed drawing. With any luck all the dimensions will update to reflect the new part geometry. Any ones that are brown or tan lost there way and will need to be recreated or reattached.

Do not try to copy assemblies with windows explorer unless you pack and go the assembly or drawing.