Sure this has been here b4 but here I go again...

Which file do I need to hack to add some default information to the hole
wizard callouts placed on prints..

My machinist would like to have the drill size I.E. 7/16, Q, etc on the
print when there is a tapped hole. I don't mind having this and have been
adding it manually.. to much work, but need to keep the machine people
happy.. I was there at one time.

Is there a data file I can add this info to so I don't have to keep adding
it for each print?

stubs,

On Feb 25, 9:15 pm, "st" <no...@nowhere.com> wrote:

Stubs,

C:\SolidWorks\lang\english\calloutformat.txt. I suggest backing it up
before changing.

Reaper.

Reaper,

I don't think there is a parameter to give numbered or lettered drill
sizes. Only the nominal drill size. I suspect the reason why is implicit
below.

Stubs,

Every other machinist on the planet can use a drill size chart. You might
let them know that we think you have lazy / incompetent machinists now.

Furthermore, it's bad, possibly incorrect, drawing practice to specify how
to make a feature unless there is a special need to specify the process.
The drawing should only specify size and tolerance. Specifying the letter
size is specifying which tool to use.

I'm all for making life easy for the machinists, but this is going too far.
Someone has to look up these brain damaged lettered sizes on a chart, and
from what I've seen, it has always bee nthe man at the machine. There is a
possibility that I haven't seen it all though.

Stubs,

You putting drill size on the prints is an unnecessary opportunity for
error to creep into your process. Also on a 1/4-20 thread a #8, #7 or
even 13/64" drills could possibly be used depending upon a few
variables in the shop that you have no control over. Then take into
account that cut taps and form taps require different hole sizes.

If you are dimensioning cut taps what happens down the road if your
company decides to use form taps? What happens if they decide to use
form taps on some materials and cut taps on the balance? Don't think
it is the machinist who will have to revise all those drawings.

IMO Prints should have dimensions and tolerances for the part and
Manufacturing/Machining then decides how best to make it. If they are
working with CAM then that program should output the machine tool
setup sheet with all the tool information needed. If they can't
configure the CAM program to output the drill number/letter/fraction
they can always input the information into a note field and output
that information in the job setup sheet.

Kudos to you for wanting to be a team player and make life easier for
others, however in this one case IMO they may not be looking at the
overall picture and it may very well come back to bite you in the ass
later on down the road.

Tom

On Feb 25, 6:15 pm, "st" <no...@nowhere.com> wrote:

Your machinist is lazy or is trying to keep you out of his hair by
making you waste time. Tell him you are not going to waste your time /
clutter up your prints with fucking bullshit. If you want to be nice
offer to order him a tap drill chart and for form tapping get him some
charts from Balax. If he doesn't like that tell him tough shit.

Jon Banquer
San Diego,CA

The parameter for the fractional, number or letter size in a Hole
Chart/Hole Callout from a Hole Wizard hole is <hw-fstsze>  I use it
all the time in my hole charts.

From the very bottom of the calloutformat.txt file.......

*Valid Hole Wizard variables are as follows:
*VARIABLE   DESCRIPTION*
*<hw-type>    Type
*<hw-std>   Standard
*<hw-fsttyp>  Fastener Type
*<hw-fstsze>  Fastener Size
*
*<hw-cbdepth> Counterbore Depth
*<hw-cbdia> Counterbore Diameter
*<hw-cdrlang> Counterdrill Angle
*<hw-cdrldepth> Counterdrill Depth
*<hw-cdrldia> Counterdrill Diameter
*<hw-csang> Countersink Angle
*<hw-csdia> Countersink Diameter
*<hw-depth>   Depth
*<hw-diam>    Diameter
*<hw-drlang>    Drill Angle
*<hw-endcond>   End Condition
*<hw-fscsang>   Far Side Countersink Angle
*<hw-fscsdia>   Far Side Countersink Diameter
*<hw-headclr>   Head Clearance
*<hw-holedia>   Hole Diameter
*<hw-holedepth>   Hole Depth
*<hw-mjrdia>    Major Diameter
*<hw-midcsang>    Middle Countersink Angle
*<hw-midcsdia>    Middle Countersink Diameter
*<hw-minordia>    Minor Diameter
*<hw-nscsang>   Near Side Countersink Angle
*<hw-nscsdia>   Near Side Countersink Diameter
*<hw-tapdrldepth> Tap Drill Depth
*<hw-tapdrldia> Tap Drill Diameter
*<hw-threadang> Thread Angle
*<hw-threaddepth> Thread Depth
*<hw-threaddesc>  Thread Description
*<hw-threaddia> Thread Diameter
*<hw-threadseries>  Thread Series
*<hw-threadsize>  Thread Size
*<hw-thruholedepth> Thru Hole Depth
*<hw-thruholedia> Thru Hole Diameter
*<hw-thrutapdrldp>  Thru Tap Drill Depth
*<hw-thrutapdrldia> Thru Tap Drill Diameter
*
*<hw-descrp>  Description

Cheers,

Anna Wood

Whoops check that.... I do not put the tap drill size in the hole
chart.  Our machinists know that info of the top of their head, we
don't need to tell them that.  Might be offended if we engineering
types tried to tell them how to do their job.....  :-)

There is a variable in the list below called <hw-tapdrldia> Tap Drill
Diameter which if you want can be added to the calloutformat.txt file
to control how your hole callouts are presented in a hole chart or
hole callout.  It probably only presents the decimal equivelant
though.

Cheers,

Anna Wood

On Feb 26, 10:05 pm, Anna Wood <a...@acrodesigns.com> wrote:

On Feb 25, 6:15 pm, "st" <no...@nowhere.com> wrote:

Stubs,

I agree with the others.  It is not only unnecessary to put the drill
size ID.  It is actually unnecessary to even state the drill size
diameter itself.  This is in accordance with a certain interpretation
of ASME Y14.5M-1994 which includes the understanding that it is
improper to over-specify a part, and improper to define processes on a
drawing.  Another reason is that if you do over-specify, you limit the
machinist choices (as stated before).  Even another reason, is that
the more information you add the more chance you have at introducing
error (typo or mis-info).  All you need to callout is the thread
itself.  In the rare event one finds it necessary to define drill
depth, simply add a statement about such without stating drill size.

2X 8-32 UNC-2B DEPTH .165

-OR-

2X DRILL DEPTH .190
8-32 UNC-2B DEPTH .165

-NOT-

2X .190 DIA DEPTH .190
8-32 UNC-2B DEPTH .165
Matt Lorono
http://sw.fcsuper.com
http://www.fcsuper.com

All,

Well these are all good reasoned logic and I thank you. I do agree that a
good machinist can call up the drill size for a 'standard' tap from memory.
I can still do almost 95% and it's been a few years. BUT,

I did inherit this Solidworks setup from the previous engineer so maybe it
is setup wrong. The 'default' way this dimensions holes from the hole wizard
is::
2x @ .201 dp .750
1/4-20 UNC dp .500

What I've been adding..
2x @ .201(#7) dp .750
1/4-20 UNC dp .500

What I would like:
2x @ .#7 dp .750
1/4-20 UNC dp .500

I was looking for a way to setup Solidworks to do this for me.

Not only does my machinist see this as a specified size for the drill it
also closes the tolerance factor to a point where he wonders about reaming..
Seems weird but there it is. I also have had outside vendors question me if
' do all these dimensions have to be three places..?'
Guess I'm surrounded by idiots..

I don't mind the drill size being called out, in fact I like to have it on
the print. It does let the machinist know what to use and what I want it
drilled at.

 I work in a small support shop that builds and maintains production
machines for a manufacturer. I rarely have to send anything out. If I do
most for the time it's to one or two tool and die shops that can and will
get down to four place decimal tolerance machining even if I give them a
fractional dimensioned drawing on a napkin... Old School Machine Work..

Thanks for the suggestions, will keep looking..

stubs

A good machinist uses the tolerance to his advantage enabling him or
her to get the work done faster. Machinists like you describe would
never make it in the shops I have worked in. They would be too slow
and cost the shop too much money.

Jon Banquer
San Diego,CA

On Feb 28, 4:37 pm, "st" <no...@nowhere.com> wrote:

Studs,

If you are making process drawings for a shop in-house, then I can see
why you might wish to add this kind of information.  With that said,
even on process drawings, it still is bad practice.  If you are
invoking ASME Y14.5M on your drawing, you are in violation of that
standard (oh the horror of it all!). ;)  Seriously though, calling
this out is a bit like calling out "FORM THIS PART WITH LATHE AWD IN
THE CORNER OF THE MACHINE".  It's not appropriate.

Each way, I do believe Anna answered your question in-directly.  I do
not believe SolidWorks has an automatic method to insert the tool
information into your callout.  Although it does know drill sizes, it
doesn't provide them to you in a callout of threaded holes.  You could
create a macro that does this for you at the end of a drawing
preparation.  You would need a table, like in excel or csv file as a
look up table.  And also, you'll need to know how to traverse through
the drawing with SelectionManager.

Best of luck!

Matt Lorono
http://sw.fcsuper.com
http://www.fcsuper.com/swblog