Handy Features to Have on Drawing Templates 1

[ZachP]

I have a bit of an exciting opportunity. My small, young company is re-doing its drawing templates. I'd like to take this chance to get the templates to be as useful and complete as possible.

We already have the basics, e.g. tolerance block, "Where Used" table, etc.

What I'm looking for is clever little things like having a "Finish" box, where one would put a flagnote if a finish is to be applied or a dash if the part is unfinished, so the reader immediately knows whether the part has a finish applied to it and where to look for it, instead of skimming through all of the notes looking for a finish (or lack thereof).

So I'm asking the peanut gallery: what are some neat, maybe not conventional, features that you've seen on drawing templates?

 

[KENAT]

I'd tend to KISS and take a good look at relevant standard such as ASME Y14.1(M).

What's great for you may not be for other drawing users and vice versa, i.e. what's useful to engineering may not be useful to the machinist, or inspection, or purchasing or....


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[randomdrafter]

If you have tool available to pull data from CAD model you add Material/Weight and other attributes automatically.

Another option we use is add is if there is any critical dimension in particular sheet.

 

[CheckerHater]

You forgot to mention what system you are using.

Some nice-to-implement features are unique to particular systems.

Also, what is the main area of your company's interest - would you benefit from creating, say, specialized templates for plastic, sheet metal, etc.?

"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future

 

[dgallup]

Assuming you are using one of the mainstream solid modeling programs, you want parameters in the model to fill in as much of the title block as practical. All the default tolerances (linear, angular, surface roughness, break edge, etc.), material spec, heat treatment and finish (paint, plating, etc.). We also use a FORM parameter which can be sheet, bar, etc. but in many of our parts will be a forging, casting, fine blanking, etc. in which case the value is the part number the finished part is made from. I also like having the CAD system and model name in the title block. We have many different product lines, some came from acquisitions and thus we use multiple CAD systems.

One thing I don't like that the OP mentioned is a "where used" block. Unless absolutely everything you draw is a one off special and will never be reused, this can never be up to date. We reuse components ALL THE TIME. I'm still using parts I drew 30 years ago in new products that I could never have imagined when the drawing was created.

/rant on/

We do use special characteristic symbols per TS16949 but those don't go into the formats as different customers have different symbols and then we have our own for internal documents. What a stupid "standard" to mandate the use of special characteristic symbols and then not define the symbols. I could see them grandfathering in old symbol sets but they could at least define a common set going forward!

/rant off/

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The Help for this program was created in Windows Help format, which depends on a feature that isn't included in this version of Windows.

 

[ewh]

I agree with avoiding a "where used" block as it can be limiting and a challenge to keep properly updated. I have seen a "First Used" block used to good effect, but this would not be a self-populating parameter.

"Know the rules well, so you can break them effectively."
-Dalai Lama XIV

 

[TheTick]

Sometimes I add a "similar to" note. That saves time for lots of people.

 

[ZachP]

Thanks for all of the replies!

To expand on the posting, we're using SolidWorks 2013, mainly for sheetmetal and machined parts, mostly aluminum. Industry is aerospace.

I like the idea of getting rid of the "Where Used" block. The company is still in its infancy, so we haven't had any headaches keeping these up to date yet, but that will be changing.

I'm hesitant to put a calculated weight on a drawing, since it is at best an approximation, and at worst totally inaccurate. For example, I've seen downloaded hardware that comes in weighing tons instead of ounces if you forget to check/change the units & properties, totally wrecking any calculated weights or CGs.

 

[drawoh]

ZachP,

"Where used" is dangerous. You have to keep this up to date. I tried "Designed for", but our documentation person claimed that had to be kept up to date.

I had this opportunity something over fifteen years ago. My idea was to have add-on sections for the title block. The main block had the title, drawing number, revision, pages, company logo, signature section, a place for stamps, and a copyright message. We have separate blocks for metric fabrication, inch fabrication, assemblies, and a projection and scale block. This leaves us with a minimal size title block, when we don't need the other stuff. It also makes for a logically organized page. For example, the scale is not down next to the page number. It is up at the top left hand corner of the block, in large font, where you actually need it.

--
JHG

 

[CheckerHater]

Agree with others on "Where used" - it's outdated. If it is an issue of great importance, invest into PDM.

It is not impossible to keep your units under control - maybe it's a matter of discipline.

Make sure you use SolidWorks Property Tab Builder to organize your file properties.

"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future

 

[Gilmiril]

If a calculated weight appears on a drawing, then the reviewer and/or approval need to check that this is correct. Just say'n...

 

[looslib]

Calculated weight should not be an issue with a solid model based system.
We give the default start template part a density of 99lbs/cubic inch. This sticks out immediately if the engineer has not set the material properties and density. The weight on the drawing will also give someone an idea if the part can be moved by hand or if they need a crane/forklift. If possible or if needed, make the parameter adjustable so you can see the weight of very small parts. We have the weight field set to display 1 decimal point value (16.4) but sometimes on small parts we get 0.0 on the drawing.
Drive a raw material block/information from part parameters to the drawing, too.

"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[imcjoek]

Calculated weight gets a bit weird if you are modelling a purchased component or otherwise simplifying the internal guts of something.
Example: A 3d model of a motor will not have a remotely correct weight unless the designer went in a hollowed it out to match the catalog spec.

 

[drawoh]

imcjoek,

Alternately, you can adjust the density. In SolidWorks, you can just tell it what your part's mass is.

Making mass correct at the assembly level is very much more important than making it work on spec. controls.

--
JHG

 

[ewh]

Adjusting the mass of a purchased component is easy... getting the correct CG can be a different beast.

"Know the rules well, so you can break them effectively."
-Dalai Lama XIV

 

[randomdrafter]

Not sure how it works in Solidworks, build a material library. Easy to apply/change materials.

 

[drawoh]

randomdrafter,

SolidWorks' material library changes the section view crosshatch. I hate it.

--
JHG

 

[Tunalover]

Don't forget the company CAGE code (formerly FSCM number). I agree to leave off the Where Used table. That information is already stored in your business system.

Tunalover