Connector Hole Layouts. BEST METHODS??

[ongybill]

I draw a lot of electrical boxes/connector panels.

Example: A 9 pin connector requires a round .813" hole with 4 holes in a .97" sq pattern centered on the circle. These 4 holes need to either be .159" if tapped 10-32, or .201" if clearance (depends how the connector is attatched).

? Is there a good way to insert the hole layouts required for ea connector w/o having to draw or transfer 5 holes each time a connector is used? Some way to use the hole wizard or something?

Appreciate any help.
Bill

 

[SBaugh]

Other then the fact you asking what are the best methods for making a hole pattern, I need to know what types of holes. Hole Wizard holes (Tapped). Normal cut holes. Linear pattern, circular pattern. I think more information is needed to give you an accurate answer.

If your in an assembly:
Hole Series



SW provides this in their Electrical package which is a separate add-in



We have a Customer and all they mostly do is Connectors, etc... They do this day in an day out.



Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
faq559-716 - SW Fora Users

 

[MadMango]

Library Features? Look in SW help.

[green]"I think there is a world market for maybe five computers."[/green]
Thomas Watson, chairman of IBM, 1943.
Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[meintsi]

Mango hit it.
Sounds perfect for the LIBRARY.

Remember...
[navy]"If you don't use your head,[/navy]
[navy]your going to have to use your feet."[/navy]

 

[Heckler]

Library Features will make it easy for you insert different connector cutouts. I also design "black boxes" and use a mixture of mil spec and commerical connectors....I create the cutout once and store it as a library feature for use on another project...

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 2.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NIVIDA Quadro FX 1400
o
_`\(,_
(_)/ (_)

Do you trust your intuition or go with the flow?

 

[ongybill]

Thanks MadMango, I was able to get that to work. I now have a library feature for creating 9 pin conn holes.

Scott. For different things I would need all of those you listed. Circular patterned holes for fan, filter, & motor mounts. Rectangular holes & hole patterns for large Electrical connectors. Round hole in the center of a sq pattern of bolt holes for round plastic connectors. Linear pattern for mounting extrusions. Offset hole pattern for mounting a flow meter we use all the time. Ect. Lots of standard components we use, it'd be nice to make patterns for the more common ones. Hope that's enough info.

MM's library features tip allowed me to size the holes as tapped or clearance, but they aren't tapped holes (ie hole wizard). Be interested to know how I can have them be actual tapped or cl holes then I could use smart fasteners & quickly add connectors.

In case it's important: Here's what I did. I created a sketch, then made 2 configurations, ea w/ 5 holes (1 w/ tapped hole size, 1 w/ clearance hole size). Then saved it as a library feature. Next I inserted the sketches where I wanted them on the part surface, then extrude cut them. Is that the right way?

Scott. Looking at the hole series command in the help it doesn't seem to apply here. Mostly I'm looking for mounting a component to a surface, not putting a hole through multiple parts. Hole series looks more useful for something like putting a long bolt or axle through several components.

 

[Heckler]

Adding onto this - I have a huge library of panel cutouts I use on at least every project...DB9's, DB25's, MIL 38999 connectors, and other industrial NEMA rated connectors. It makes creating an interface panel a snap....read up on this and truely experience the real power of SWx. Don't forget we will be here to help you along the way.

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 2.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NIVIDA Quadro FX 1400
o
_`\(,_
(_)/ (_)

Do you trust your intuition or go with the flow?

 

[ShaggyPE]

ongybill,
you can have more than one feature "stored" in a library feature.
Example:
for a DB-9 connector, you would have a sketch of the D shape. Your second feature would be a hole wizard hole on both sides of the cutout. Both of these features would be part of the library feature.

Once the library feature is inserted into the PART model, it can be patterned using the pattern feature command. Going this route, you can populate all the similar connectors in your assembly by simply mating one connector to the first cutout you made. Using insert>component pattern within the assembly you will be able to populate all the other cutouts.

 

[ShaggyPE]

Also, after re-reading your post about inserting the sketches into your new part. It didn't sound like that was done properly. You shouldn't be inserting sketches, you should be inserting a library feature.

This is done by going to insert>feature>library feature.

When it is inserted, an icon in the feature manager design tree will appear. It looks like a stack of books. The plus sign next to the books will allow you to expand and change the internal features.

It really is a great functionality for standardized cutouts.

 

[ongybill]

You're right I was putting the sketch on the part, then extrude cutting it, which worked, even if it's not the best method. Didn't realize I should be putting the features (holes) in the part. I tried for 1/2 hour or so this morning to get it to work as a feature that'd insert w/ zero success. But, haven't been able to do anything with it since (deadlines). Perhaps I made it too complex trying to use the hole wizard (as Scott alluded to). I'll try it later just using circles.

{This is done by going to insert>feature>library feature}

Couldn't find this under the insert menu, or in the help files. Where is it?

The help files say to drag it from the library to the part you want the holes in. Which put the sketch on the part, but didn't add any holes (not sure why yet).

Anyway thanks. Once I figure out how to make this work it'll save me tons of time.

 

[Heckler]

Do a search in the help file for Library Features....they're stored in the design library which is the tab to the left or right on your screen (if you have it activated)

{This is done by going to insert>feature>library feature}
might be a 2003 or 2004 command structure.

So save your library feature to the following path

C:\Program Files\SolidWorks2005\data\design library

Then you should be able to insert them through the design library. SWx has made inserting a library feature extremely easy compared to past releases.

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 2.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NIVIDA Quadro FX 1400
o
_`\(,_
(_)/ (_)

Do you trust your intuition or go with the flow?

 

[J-C]

If you are on subscription support, download the beta for 2006, there might be some surprises there. While it's beta and that won't do you much good now, release should only be about a month away.

Jason Capriotti
Smith & Nephew, Inc.

 

[ongybill]

Still can't get the feature to insert into the part.

Pretty easy to draw it and save it to the library. But only the sketch transfers, not the hole feature.

I've followed the directions in the help file (drag the features not the base part to the library window then assign it a name). Plus as many variations as my fertile imagination can come up with, but why no matter how I draw the holes in my base part; or how I save it; they won't transfer as holes to the part I'm trying to use the library feature in???????????????????

I've tried everyway I can think of. Looked at the existing hole pattern files. Ect.. Can't see where the existing files do anything different, except they work and mine don't.

What am I missing, this'd save me tons of time if I could only figure out how to use it.

 

[SBaugh]

1) Make a base part
2) make a feature
3) Highlight the Feature
4) File/Save as/Library part (browse to location)
5) save file.

Make a new part and if your Library feature is saved in the right location it will show up in the Task pane, under Design Library. Drag and drop the feature into your new part.

See if that helps, If not I will make an Movie file tomorrow or the next day.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
faq559-716 - SW Fora Users

 

[ShaggyPE]

Heckler is correct that my comments are based on 2004. My company is still in the stone age (lol). Hopefully the interface has not changed such that this comment is totally irrevelant, but here goes.

ongybill, you should be able to have multiple features including hole wizard holes tied into one library feature. A library feature used to be created by saving the part model as a Lib Feature Part (.sldflp). Prior to saving the model, I cntrl-selecting all of the features that you want lumped into the library feature. If you want to add more later, you can right click on the feature and "add to library". You will notice the icons in the feature tree change.

The steps using SW2005 may be different but I am willing to bet that the general principal is the same (dragging the features to the design library sounds pretty similar to saving the features as a Lib Feat Part).

The old (as I described) method may still be available, you may still want to give it a try.

 

[ongybill]

Thanks Scott & Shaggy.

It works great if you select the feature and then saveas library feature. Pretty simple too.

The help says to select the features and drag them into the design library window. That saves it, but the features don't work.

Pretty slick. Once I get enough hole patterns drawn that'll save me tons of time.

Have a good weekend.

 

[SBaugh]

The Drag was put in at SW05. I'm a bit old school and I still save mine that away.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
faq559-716 - SW Fora Users

 

[ongybill]

Well Scott,

From my limited experience the drag feature doesn't work anyway. At least not in SP0.

Thanks for the help, that's a great feature that'll save me tons of time once I get some library features built.

Now I'd best get some work done. Got a project due Wendsday that I need at least till Friday to finish. Usually that when my boss shows up with a concept drawing he needs done RIGHT NOW. LOL He has a 6th sense.

 

[ongybill]

Scott

Thanks for turning me onto the hole series command. Just used it to punch a grommet hole through some seperated panels.

Related question. I punched the holes, then inserted a grommet (part) into ea. hole. Then when I went to unhide a bunch of parts I could only select 1 at a time (too time consuming with 30 hidden parts). This happens occassionally. The only way I've found to be able to select a string of parts to hide/unhide again is to close the file and reopen it. Then it works fine. Just an SP0 bug?

 

[SBaugh]

Crtl-Select each one or if they are in a row hold the shift key and select the first one, then the last one in hte list, This will select all the parts from there.

Also look at Edit\Show with dependents then pick the appropriate option from there.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
faq559-716 - SW Fora Users