Lenght in BOM 1

[andrzej01]

I use part in the assy which is made by sweeping profile along path.
I would like somehow to show length of this sweep in feet in BOM.
Is that possible at all?
Andrzej

 

[MrPickles]

If your sweep is a true curve, you can get the length of the curve and assign to a Property. Otherwise, I use a construction line in a sketch, use equations to calculate it, and use that in a Property.

Mr. Pickles

 

[SBaugh]

If you dimension controlling the length. Then you can go to the custom tab under File\Properties. Type in a name like Length and double click feature in FM then double click the length dimension. Click OK and you know have a custom length property that can be placed in you BOM if your BOM is set up correctly.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
When in doubt, always check the help

 

[TheTick]

FYI--If you are modeling in units other than feet, you can change the units of individual dimensions. This may help in concert with the other suggestions above.

Good and evil: wrap them up and disguise it as people.

 

[TheTick]

One more thing...

http://www.eng-tips.com/faqs.cfm?spid=559&sfid=590

 

[brengine]

I don't remember where I found this, but maybe it'll help:

You can get the length of a part into the description as follows:

Start your custom properties editing in the part as usual with File, Properties. Then switch to the 'configuration specific' tab and select the 'description' property (or whichever you use in your BOM description field. In order to get values from annotations, type in the text portion, then double click your part (with the property dialogue still open) and click the text of the annotion you want. So, for example, you can type:
'ALUM. EXTRUSION, '
Then select from your profile sketch an overall dim showing the extrusion size. Next you type:
'MM SQ. X '
Now you can select the extrude length dim. Finally, finish it off with your desired text at the end, such as:
' MM LG.'
Remember to click Add or modify!
When you select the dims, Solidworks automatically puts code in the property which reads the value. You will see something like
'"D1@Sketch1@@Default@Part1.Sldprt"'

The entire File Properties will look something like:
ALUM. EXTRUSION, "D2@Sketch1@@Default@Part1.SLDPRT"MM SQ. X "D1@Base-Extrude@@Default@Part1.SLDPRT" MM LG.

When the BOM reads the property from the example above, it will show:
'ALUM. EXTRUSION, 40MM SQ. X 232 MM LG.

 

[StarrRider]

KenBolan

I love it – Very good tip. I learn something new every day. Didn’t know they could be combine them like that.

Lee

Consciousness: That annoying time between naps.