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WhatÆs the quickest way to make dimensioned machining drawings? 2

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aliensquale

aliensquale

Mechanical
Oct 20, 2008
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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.
 
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Do a file, save as, choose new location, new name, then...
click the "reference" box and edit (slow double click) the model path and file name, select ok (that menu will be updated and close), select "save" and you have:
A new drawing, a new model in a new location.
 
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Actually i do know how to use solidworks explorer. Hence my statement.

If he is commenting on the difficulty with just creating a drawing do you think it is wise to recommmend using another piece of software?

Often times training someone requires understanding the current process they are using and assisting them with being effective under those methods.

Then and only then slowly show them the benefits of productivity tools geared towards specific products.


 
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I remember a quarter of a century ago when AutoCAD first appeared some people where complaining that it takes so much longer to create drawings with AutoCAD than by hand on the drawing board. Can you believe that?
 
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"It sucks." Why? What about it sucks? We use SW Explorer to copy many parts and assemblies each day, and it works very well. I've yet to run across a problem when I use the utility correctly.
 
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aliensquale said:
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.
Click to expand...
next breath
aliensquale said:
I know solidworks explorer, and I have to agree with the prior poster, it sucks!!!
Click to expand...

Pretty bold statement. I use SWExplorer all the time and prefer it over save as in most situations.

-Dustin
Professional Engineer
Certified SolidWorks Professional
Certified COSMOSWorks Designer Specialist
Certified SolidWorks Advanced Sheet Metal Specialist
 
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I have never used the pack and go, good point, maybe I renag my last statement, if I pack and go, then copy that to a new folder, rename the part and drawing hopefully that will do it for me. I just hope by renaming the two files the references will automatically be updated..
 
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When you pack and go, this can all be done in one step. Select the pack and go option, then click Select/Replace. In that dialog box there are many options, but you can change the save to name to whatever you choose (change the part number, for instance, in the "Replace text with" box), and it does it to all parts/assemblies/drawings that are selected.

This eliminates the need to then go in and manually change names, break references, etc. We use it daily and it saves a lot of time.
 
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The problem with save as copy is that it doesn't ever update the reference to any drawing, it just makes another dumb model.

If you use the method I mentioned of copy a "template" part and drawing into a new location, open said part in sw explorer, rename the part, then rename the drawing (this can be done in std windows explorer, because the drawing does not link to anything).

After that you have a totally autonomous new part with already detailed drawing associated with it. Otherwise you have to rename, and then go the extra mile with fixing references. Then hope you didn't accidentally change the original model instead of the new one because you messed up the 2nd step.

SW explorer is the only tool I'll use to update file references. Just get a routine down to using it and you'll be better off for it. It saves tons of time.

James Spisich
Design Engineer, CSWP
 
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aliensquale -

i'm a younger guy, working at a shop similar to yours. at first, the older guys were resistive to making the switch. they were very defensive and fought it hard. they were on Autocad13 when I came in here back in 2004. but now, they are floored by the speed, accuracy, and the ability to manipulate the drawings based on product families.

we make parts similar to yours. as mentioned above, the thing to do is make an example template drawing and part model for each product family. open the drawing first, do the save as, then open the part from the drawing (right click in one of the views), do a 'save as' on the part, then go back and save the drawing again. in the model, manipulate the revolve or hole sizes and save. do a 'ctrl+q' on the drawing and all the dimensions will auto update. i prefer this method over the 'save as copy' method.

as a side note, i would use the hole wizard as much as possible. down the road, it will make things much easier if you ever are cutting on a water-jet, laser, or use mastercam. we also put a PC out in the shop and showed the machinists how to use Solidworks viewer to spin the parts around.

lastly, i agree with what everyone mentioned above. 3D will be faster once your CAD guys have been working at it for a while. not to mention having the correct 2D sketch ALWAYS because it is based on the model, not some fudged in lines that will come back to haunt you down the road.

good luck. you made the right move.

-michael
 
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Here is a link to some pdf's of a typical toolkit I design to create the process carriers that we sell.


The tookit and its details took me about 1:45 to 2:00 hours to create. This is from the time I recieved the job traveler until I am done with a release to manufacturing control to build.

This includes pulling my part numbers, designing the tool, uploading the pdf's and solid models into our document management sytem and adding the part numbers to our ERP software.

I have maybe 45 minutes in SW time, the rest is just the rest of our engineering processes that we have to manage our work.

The carrier drawing that is in the package is what this tooling creates. I have maybe an hour in design work on that carrier.

We do lots of copy and cloning with modular tooling and families of parts/products.

When I started our conversion to SW from AutoCAD last year, we figured it would take me a year to get our product line (tooling and carriers) in good order and be able to work at the same speed/quicker as our AutoCAD work. I am as quick or better as when we did this in AutoCAD with way less mistakes in the designs.

I am an experienced SW user having worked with it since 2003. We have done all of our other tool and automation equipment design in SW since 2003. Our product line area was the last holdout, with our last designer hanging on to his AutoCAD ways of doing things.

For a company just making the switch, with no real training or experianced SW users on staff it will take time to get efficient.

The benefits are worth it but it takes a major commitment from manangement to stay the course and to take advantage of what 3D CAD can do for you.

We use all of our 3D CAD data downsteam in our CNC's, water jet, laser, QC and on our CMM's. I make renderings of our product to give to our customers and help our sales efforts.

There is many an order/project we would not get if we did not have the ability to work in 3D with solids and SolidWorks specifically.

With some hard work, creative thinking and some perserverance the transition is more then worth it.

FWIW,

Anna Wood
SW2008 SP4.0, Windows Vista SP1
IBM ThinkPad T61p, T7800, FX570M, 4 gigs of RAM
 
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