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I have a generic fastener (Rose Head Nail) that has two derived configurations. Unsure how to proceed

Question asked by Rob Edwards on Mar 2, 2017
Latest reply on Mar 3, 2017 by Rob Edwards

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I have modeled a generic Rose Head Nail. It has two derived configs - half or fully clenched.

There are so many different sizes possible, head size, shank size, length, clench position,etc that I need to create new configs on the fly. We have certain standard sizes we buy from various suppliers, we also have buckets of vintage ones in the workshop attic, but the biggest problem is the length to the bend will vary from job to job. I was hoping to use the config publisher, but that needs a 1 line design table. The derived configs, already give me 3 lines. I deleted the two derived configs in the DT and then got the config publisher to work in its alternate form of creating rather than selecting configs, but it's not able to create the derived configs

It's like I need to apply the flex in the assembly, I wondered if I should use a part in part approach. I could create all my configs of the nails we buy from various suppliers and add more as I need easy enough, insert this part into a 'clenched' part where I apply the flex to the solid body and have this part saved as a template for each new job.

Or driveworks? I get so confused sorry any advice much appreciated.

Also while I'm going to the trouble of creating these parts is it worth adding a smart feature to drill the hole, or am I better to add my nails to holes I've already created?

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Paul Risley Mar 2, 2017 3:50 PM
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Rob,

May help or not. From what you described I would not use the derived configuration for the 3 states shown. Rather I would use those as my main configurations as they are the 3 main geometrical form states.

As far as a design table or configuration publisher I would think that if you had 3 main parts

Straight

Clenched

Half clenched

It would be easy to drive your configurations at this point as each configuration could have a design parameter for it's subset rather than the software struggling against a half clench profile to a full clench profile.
If that makes sense.

Hope that helps some bit.
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- Rob Edwards @ Paul Risley on Mar 2, 2017 4:30 PM
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  Thanks Paul
  
  That sounds good. I'm pursuing my part in part approach, where I have 3 configs as you describe
  And I have my 'bought in' configs in the base part
  Seems to be working so far...
  
  edit: I spoke too soon. I was hoping that the config of the inserted part would be unconfigured, so that I could choose a config that would apply across my default/clenched configs but I find no way to do this. Still it's better than anything I've had before
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Vladimir Urazhdin Mar 2, 2017 4:17 PM
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I had a similar problem with configurations + variable dimensions driven by top level dims. My solution was to create a minimum required configurations + add a Global Variables for each configuration, linked both to variable dimensions on a Part Level and Top Level Assembly (dimensions or/and Global Variables).
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John Stoltzfus Mar 2, 2017 4:25 PM
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Over the years I have done quite a bit of Design Tables - some good and some not so good... But this would be a perfect setup for a good design table setup. The reason I like to go that direction is you can very easily add additional rows in the excel spread sheet, plus you can add all the custom properties so they stay with the part. Plus when your in the middle of a design and you need one that is 5mm longer, no big deal it's there and if not, it doesn't take long to add one.. Eventually you may want to consider inserting them in Toolbox...
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- Rob Edwards @ John Stoltzfus on Mar 2, 2017 4:44 PM
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  Thanks John
  Yes I'll make a DT - I love Excel - but I wanted to start right before I populate it all. I've never used Toolbox, I just checked
  Is it included as standard?
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  - John Stoltzfus @ Rob Edwards on Mar 2, 2017 4:55 PM
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    Did you do design tables before?
    
    Attached is a small file
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    SHCS 5-16-18-BL OX_.SLDPRT.zip2.7 MB
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    - Rob Edwards @ John Stoltzfus on Mar 2, 2017 4:58 PM
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      Thanks John, I'll take a look tomorrow, I just noticed the time, nearly 10pm here I should go home
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    - Rob Edwards @ John Stoltzfus on Mar 3, 2017 5:49 AM
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      Morning John
      Sorry I can't open your file - I'm stuck back in 2015. I would be very interested to see how you order things in your DT. Please if possible, could you send me just the DT, it's only half the picture I know, but I don't think I've ever seen a proper one made by a pro
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      - John Stoltzfus @ Rob Edwards on Mar 3, 2017 6:20 AM
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        For earlier versions go to 3dcontentcentral.com and type my name in the search bar, then down load one of the sprockets or whatever else you want, make sure you have the "All Configurations" checked and also which version you need, then open the file and edit the Design Table.
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  - Rick McDonald @ Rob Edwards on Mar 2, 2017 6:31 PM
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    Rob Edwards,
    unfortunately, no - TB is not included with Standard - (one of the main reasons WE don't use it).
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    - Jim Steinmeyer @ Rick McDonald on Mar 3, 2017 10:39 AM
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      From experience, that is NOT a bad thing.
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Rob Edwards Mar 3, 2017 9:35 AM
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An update on what I have done

Created Base Part of the nail, with configs of Nails as we buy them in, added a DT and Config Publisher
Inserted Base Part into new part that applies the flex (no configurations)
Popped both parts into a New Folder in my Library.

My proposed workflow
If I need a straight nail just drag it into the assembly and choose the config
If I need a clenched nail, drag it into the assembly, make it a virtual part to break links, choose config via external references, adjust the sketches to be parametrically linked to the new assembly and save it out.

comments:
Even when using derived configurations, the default behaviour of the configuration of the inserted part is configured, not linked to parent (as I would assume)
When the configuration of the inserted part is changed, SW does not rebuild equations, so it created errors in my flex feature.
My solution was to remove equations and use sketch relations (which do update) to hopefully minimise errors.
It would be nice if it was possible to make it smart, so that I could drag in a clenched nail, select a couple of faces and have the nail adjust itself, but this is a big improvement on anything I've had before.

I'm looking at doing a similar thing for other hardware now, I feel like I'm at the start of a long road, so your comments are truly valued
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- Rosehead Nail.zip547.5 KB
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- John Stoltzfus @ Rob Edwards on Mar 3, 2017 9:48 AM
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  Thinking about your project a little more, here is what I would do..
  
  Make three parts - Straight Nail - L-Nail - U-Nail all different files
  In each model create a design table for the different sizes -head or shank or length would be the only features that you would use in the design table.
  In each model create the same position Mate References, get creative here and visualize how you would typically mate these Nails, add Surfaces or Sketch Points and use them for References
  Basically you could setup one file and make sure it changes size the way you need it to and then do a "Save As Copy" for the other two Nail Configurations and then add the additional boss or cut extrudes etc.
  
  The advantage of doing it this way is to keep the file size a lot smaller, but the biggest reason is changing out components utilizing the "Replace Components" feature. I am assuming that your assembly will have either Straight or Clinched nails, but if you need to change out to another style of nails it is easy to highlight the Nails in the Feature tree and right click and replace components, pick out the one you want and viola - you done...
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  - Rob Edwards @ John Stoltzfus on Mar 3, 2017 10:14 AM
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    Yes
    
    The nails will be either straight or clenched, but they would be the same 'actual' nail, so that is what I want in my BOM.
    I anticipate that in either case the size of the nail will have to change, for example in a door assembly, the nail config will change as the door gets thicker.
    With regard to mate references I've already included a sketched circle, to coincide with a hole on the face, but I'm not 100% how to set them up properly. I'll have a play with that now.
    A lot of the time they will be patterned. We use them for everything, from pinning on an escutcheon, nailing on penny-end hinges, actual door construction itself or nailing down a floor.
    It would be nice if the nail could size the pilot and clearance holes required, instead of the other way round.. is that where you would use a smart feature?
    
    I like the idea of using replace components, but I'm not sure why I would want 3 separate files and DT's. At the moment there is just 1 DT so I can easily add in a new nail as I need it, but I take heed and will keep a lookout on the file sizes.
    
    Again thankyou so much John
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    - John Stoltzfus @ Rob Edwards on Mar 3, 2017 10:47 AM
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      Sure you can use the same file for all three , just makes the design tables much easier if it's only a few sizes you need to deal with, especially down the road you want to add a new size, now you have to make sure which features to suppress or un-suppress ect....
      
      You can use the nail to drive the hole size if you edit the board and use the Cavity Feature and a small round clearance extrude in the nail, which brings me to another question? How much of the nail do you "Show" the customer in the Design Model or Drawings, do you show the drawing with Hidden Lines shown, if not then I would re-model the Nail so that you can use the nail shank to drive the hole size, so all you would see is the head and a straight round extrude and the bent nail you would show the head and the clinched part only, the rest would be a straight round extrude as well, now you can use the cavity feature with ease.
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      - Rob Edwards @ John Stoltzfus on Mar 3, 2017 10:39 AM
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        Ha! You're spot on there. As far as the customer is concerned, its mostly cosmetic , it's the QTY that's important in the office and the holes on the shop floor. You're keeping me busy John
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        John Stoltzfus @ Rob Edwards on Mar 3, 2017 10:49 AM
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        Which would make your nail look like this
        
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        Rob Edwards @ John Stoltzfus on Mar 3, 2017 11:00 AM
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        As Im putting a square peg in a round hole so to speak, maybe I could have the best of both worlds, retain the square shank and have an additional cylinder body to make the hole?
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        John Stoltzfus @ Rob Edwards on Mar 3, 2017 11:03 AM
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        If your square shank is bigger then the round shank then the cavity feature will create a square hole, ok if that's what you want
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        Rob Edwards @ John Stoltzfus on Mar 3, 2017 11:31 AM
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        John Stoltzfus @ Rob Edwards on Mar 3, 2017 11:33 AM
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        Not sure where your getting that icon from - You need to "Edit" the board that it's going into and then select Cavity
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        Rob Edwards @ John Stoltzfus on Mar 3, 2017 12:08 PM
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        Thanks for bearing with me John, I got it. I never used Cavity before, I normally use indent
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I have a generic fastener (Rose Head Nail) that has two derived configurations. Unsure how to proceed

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