Hole Callouts & Bolt Circles

[mwa...@my-deja.com]

I know there must be a way to reference the BC diameter of a hole (as
well as the number of holes) in the hole callout such that if I change
my bolt circle and/or # of holes the callout will automatically update
Can anyone explain how to do this?

thanks in advance

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[Jim Sculley]

mwa...@my-deja.com wrote:
>
> I know there must be a way to reference the BC diameter of a hole (as
> well as the number of holes) in the hole callout such that if I change
> my bolt circle and/or # of holes the callout will automatically update
> Can anyone explain how to do this?

I don't think it is possible. It would be nice if you could reference
dimensions similarly to the way you create symbols:

<MOD-DIAM><DIM> THRU
2 PLACES 180<MOD-DEG> APART ON A
<D1@Sketch2> BOLT CIRCLE

Something like this would solve the chamfer dimensioning problem as
well. If there is a way to accomplish it, I haven't found it.

Jim S.

[mwa...@my-deja.com]

It seems like it should be in there somewhere. Its such a necessary
option, as i often find myself redesigning and forgetting to change my
callout. little mistakes like that can end up costing thousands or
more...

thanks anyway

In article <3A6DC168...@abraxis.com>,

[Jim Sculley]

mwa...@my-deja.com wrote:
>
> It seems like it should be in there somewhere. Its such a necessary
> option, as i often find myself redesigning and forgetting to change my
> callout. little mistakes like that can end up costing thousands or
> more...

Yup. You are in the same boat for chamfer callouts, which must be added
as a note, and cosmetic threads callouts which import as notes. There
may be others, but those are the three that cause me the most grief.

Jim S.

[dv...@my-deja.com]

Hey guys,

You can accomplish this task with SW2K1 very easily. Inside the part
file with the dimensioned chamfer feature. Just make a new custom
property say, Chamfer-1, and copy those dimension names in.

For Ex:
"D1@Chamfer1@Part1.SLDPRT" x "D2@Chamfer1@Part1.SLDPRT"

Then, in your drawing you just and the chamfer note and grab this model
property and add the correct symblos such as:

$PRPSHEET:"Chamfer-1"<MOD-DEG>

That should work, and it WILL UPDATE when a dimension is changed in the
part file. COOL

That should save you guys forgetting to update the old manually entered
stuff later.

Don Van Zile

In article <3A6E2A5B...@abraxis.com>,

[dv...@my-deja.com]

Sorry, I forgot to explain how to do it with the Bolt Circle.

If you read my previous thread do the same thing except use the
dimension names you get from the feature pattern. You will have to
create a construction circle (bolt diameter and dimension) when you
create the hole to be patterned. Then, just make two new properties in
the model file like so.

Property Name ----> Bolt Circle
Value------------->"D2@Sketch2@Part2.SLDPRT" DIA. BOLT CIRCLE.

Property Name ----> Number of Holes
Value------------->"D1@CirPattern1@Part2.SLDPRT" HOLES

then in your drawing with the note callout just grab these external
model properties.

Your Note should Read---->$PRPSHEET:"Bolt-Circle"
$PRPSHEET:"Num-Holes"

This Note should update when your model bolt circle changes or the # of
Holes! That will work and save many errors later too.

Don Van Zile

In article <94k9nf$vr9$1...@nnrp1.deja.com>,

[mwa...@my-deja.com]

Is this possible in sw2k as well?

i tried it and it didnt work, so if it is possible i must have done
something wrong. i dont quite understand the $prpsheet, is this a
command or is it file-specific (ie did you give this value a generic
name or is it i solidworks command).

[Jim Sculley]

mwa...@my-deja.com wrote:
>
> Is this possible in sw2k as well?
>
> i tried it and it didnt work, so if it is possible i must have done
> something wrong.

No, it won't work for SW2000, and it is a complete hack in SW2001 in my
opinion. This functionality should have nothing to do with custom
properties.

> i dont quite understand the $prpsheet, is this a
> command or is it file-specific (ie did you give this value a generic
> name or is it i solidworks command).

You use it as shown. It simply tells solidworks to look in the custom
properties for the part and grab the value from there.

Jim S.

[Scott Wertel]

I have used this technique for SWX2K but not in the part model.

When in the drawing file, import the dimensions. Create a note pointing to
the object you wish to call out. With the note (annotations) dialogue open,
double click the dimensions that you want shown in the note. Add extra
characters as necessary. The note dialogue box will display the dimension
name string, but the final note will display the value. After the note is
placed, hide the imported dimensions used to create the note...DO NOT DELETE
THEM. If you delete them from the drawing, your note will not update. If
you just hide them, the note will update.

--Scott

<mwa...@my-deja.com> wrote in message news:94mitk$ujj$1...@nnrp1.deja.com...

[dv...@my-deja.com]

Unfortunately the answer is no. SW2K1 has the new functionality that
allows access to dimensions in custom properties. Once you make these
new custom properties as discussed in the previous threads, you can use
those properties in notes on drawing sheets. That's when you will have
to use the "$prpsheet" jargon to call from these properties.

I know some of those inserts are confusing, but I’ll try to walk you
through the chamfer callout.
(Again, this “must” done in SW2001 and will not work in SW2000)

1. Start a new part.
2. Start a sketch on the front plane and sketch a rectangle say 3” long
x 2” high
3. Extrude this to about 1”
4. Next, add a chamfer feature to the now clearly visible far top right
edge.
(Say, Angle-Distance 1” & 45deg.)
5. In the feature tree, right-click on the “Annotations” and turn
on “Show feature Dimensions”
6. Now go to the “file” pulldown and click on properties.
7. In this properties dialog box click on the “Custom” tab (move box if
dims. Can’t be seen)
8. In the “name” textbox type chamfer-1
9. Next, click once inside the “value” textbox to activate (as if to
start typing in it)
10. Now, in the graphics area, click on the 1” chamfer dimension and
you should now see something like
D1@Chamfer1@Part1.SLDPRT in the “value” textbox now
11. Next, in this same text box and a space after that and an x
D1@Chamfer1@Part1.SLDPRT x
12. Now, in the graphics area again, click on the 45deg dimension.
13. You should now see
"D1@Chamfer1@Part1.SLDPRT" x "D2@Chamfer1@Part1.SLDPRT"
in the “value” textbox.
14. Now, click the “ADD” button in the dialog box to add this new
property.
15. Save this part.
16. Start a new drawing and insert the standard three views
automatically.
17. Next, bring up the “Note” (insert note) dialog box.
18. Click on the graphic icon (looks like a magnifying glass and a
folder). This bring up another dialog box from which you can grab
the “custom” properties from this part.
19. Make sure you check “External Reference” option, and then activate
the combo-box dropdown arrow.
20. You should see the “Chamfer-1” property and select it. Then click
OK to close this box.
21. Next add the degree symbol by going into the “Add Symbol” dialog
box. You should now see
$PRPSHEET:"Chamfer-1"<MOD-DEG> in the text area.
22. Now just select the chamfer edge in the graphics area and place the
note where you want it.
23. You should now see the dimensioned chamfer callout and it wil
update if you ever change these dimensions in the part file.

Don Van Zile

In article <94mitk$ujj$1...@nnrp1.deja.com>,

[Jim Sculley]

dv...@my-deja.com wrote:
>
> Hey guys,
>
> You can accomplish this task with SW2K1 very easily. Inside the part
> file with the dimensioned chamfer feature. Just make a new custom
> property say, Chamfer-1, and copy those dimension names in.

<snip>

This is hackish in my opinion. For instance, I dimension my models to 4
decimal places. My chamfer size will never need to be more than two
decimal places, and the angle will need 0 decimal places. To achieve
the desired results, I would have to individually set the dimension
precision of each dimension (about ten mouse clicks each). I can
probably automate the process with some VBA code.

While this does eliminate the problem of keeping the dimension
up-to-date, it is hardly the best way to do it.

Jim S.

[mwa...@my-deja.com]

I got it to work in sw2k. It seems pretty time consuming. Im still
trying to decide if its worth the time.

What I cant figure out is how to change the precision. i get 2 place
and i need three, all of my dimensions are i three place, but when i do
the references on the drawing they come out two place. any ideas how to
solve this?

thanks,

Matt

[dv...@my-deja.com]

Just change the precision in dimension in the part file.

In article <94mpvf$4ro$1...@nnrp1.deja.com>,

[mwa...@my-deja.com]

ugh, that was silly, my precision was on 2 place in my drawing file.
one more question on this issue: any way to get tolerances on these
values? i put the tolerance on the part file dimension, it shows up
when i insert dimensions to the drawing, but it doesnt show up on the
note?

thanks again. this has been extremely helpful.

[mwa...@my-deja.com]

That is much easier and faster. thanks alot. still cant get my
tolernaces to display, though