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Trying to figure out sub-weldments

Question asked by Mattew Stafford on Feb 13, 2017
Latest reply on Feb 14, 2017 by Deepak Gupta

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Maybe I am assuming that a subweldment should be able to do more than what it is supposed to do. I have a weldment & created a subweldment that consist of 3 parts (shown in the tan color).

1) I have created custom properties of the sub-weldment & a description called "Atmospheric Damper Take Off". This shows up as item 1.5 on the BOM.

2) I have created custom properties of the items under that sub-weldment. They do not show up. Shouldn't they show up to be something like 1.5.1, 1.5.2, 1.5.3, etc.?

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Stephen Bittner Feb 13, 2017 1:12 PM
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You should be able to configure the BOM settings to show "Parts Only".
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- Mattew Stafford @ Stephen Bittner on Feb 13, 2017 1:15 PM
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  This is what it looks like when I select "parts only". The thing is, I want to show the indented style.
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  - Stephen Bittner @ Mattew Stafford on Feb 13, 2017 1:24 PM
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    I see! I think your first picture is already "indented". I'm not aware of another way to indent it to another level.
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    - Mattew Stafford @ Stephen Bittner on Feb 13, 2017 1:40 PM
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      I guess I am confused what purpose then sub-weldments are for? I opened up the solidworks help on creating sub-weldments and I did a RMB, "insert into a new part", then saved that weldment as a new part. So I figured that I could then have an item number & description of each cut list item in this part.....Unfortunately, that did not work. I get the following message:
      My properties are linked to the original "parent part":
      Nothing shows up in this BOM either. I appreciate your help.
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      - Stephen Bittner @ Mattew Stafford on Feb 13, 2017 1:51 PM
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        I have very little experience with weldments. I prefer to create parts and sub-assemblies to create my assemblies. That said, it seems that if you saved the sub-assembly as a "Part", then it will act like a single part in the BOM?
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        Mattew Stafford @ Stephen Bittner on Feb 13, 2017 2:00 PM
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        I misspoke on my previous response. When I create this new part, yes, there is a single part in the BOM. Even though there are other parts within it. I suppose I could export the parts of the weldment into an assembly, but it sure seems like a long way to go about things, when the weldments should work properly IMO. I appreciate your help!
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Stephen Bittner Feb 13, 2017 1:59 PM
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Maybe this thread helps?
https://forum.solidworks.com/message/508211#comment-508211
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- Mattew Stafford @ Stephen Bittner on Feb 13, 2017 2:12 PM
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  Interesting! Same issue I am having. As mentioned I created a new part & the cut list items did not show up. When I import them into a new part, they show up. There must be something everybody is missing. I have to create 3 files in order to get a bill of material on a drawing that I don't want?
  1) My original file with the weldment
  2) Selected parts of this weldment "saved as a new part"
  3) New part created, only to import the previous part that was saved.
  I just want the cut list descriptions & sizes to show up on one of my sheets of my assembly drawing. Once again, I thank you for your help, but I am more confused then ever what subweldments are even for?
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  - Deepak Gupta @ Mattew Stafford on Feb 13, 2017 2:45 PM
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    Mattew Stafford wrote:
    
    but I am more confused then ever what subweldments are even for?
    Sub-Weldment are mainly to save multiple bodies to a another part (unlike when you can only save one body per part). This also enables it (and all bodies under it) to list as one single item instead of multiple in cut list/BOM.
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    - Mattew Stafford @ Deepak Gupta on Feb 13, 2017 2:58 PM
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      Thank you for the explanation. I suppose there are situations when you might want to have it listed as one single item. However, we have several drawings (autocad) of multiple smaller weldments as part of a larger weldment. Each sub-weldment may be farmed out to many different fab shops. It would be interesting to see what everybody else is doing when it comes to ballooning weldments. If there is an alternative, I would be all ears.
      In fact, I already had a similar post recently, but it would go along with this thread... Our machined parts would normally have one item number (and their own drawing) & as a component underneath that, there would be a weldment (with its own drawing). Does everyone else just detail the machined part & let the fabricator figure out how to weld it without ballooning it as another item?
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      - Deepak Gupta @ Mattew Stafford on Feb 13, 2017 3:03 PM
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        We had to deal with a similar situation and instead of using sub-weldment, we created configurations in the part model and then detailed them as separate drawings or multiple sheets. And then created one assembly (with those configurations added in without any mates but fixed) ballooning those configs/part instances. Also added exploded views, etc. This made the huge weldment drawing more cleaner and easier to read.
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        Mattew Stafford @ Deepak Gupta on Feb 13, 2017 3:30 PM
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        Hmm..trying to see if I understand correctly.
        We had to deal with a similar situation and instead of using sub-weldment, we created configurations in the part model (I have done a little with configurations, but because of the way this weldment was created, when I suppress other features, it also suppresses the part(s) I want to keep.) and then detailed them as separate drawings or multiple sheets. (I can detail them on other sheets by using model views if I want to, but I am trying to distinguish these weldments with items numbers based off the top assembly...I think this is what you are explaining next.) And then created one assembly (with those configurations added in without any mates but fixed) ballooning those configs/part instances. Also added exploded views, etc. (I will check into this tomorrow, but I didn't think your BOM could include more than one configuration. Unless you are saying that your assembly included overlaying the same files on top of one another, but with different configurations.)
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        Deepak Gupta @ Mattew Stafford on Feb 13, 2017 3:38 PM
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        Mattew Stafford wrote:
        
        I have done a little with configurations, but because of the way this weldment was created, when I suppress other features, it also suppresses the part(s) I want to keep.
        Use delete bodies and not suppress.
        
        I can detail them on other sheets by using model views if I want to, but I am trying to distinguish these weldments with items numbers based off the top assembly...
        When broken down into conflagration, the number of bodies would be reduced. So simple take (assume) each configuration as separate part/weldment and detail.
        I will check into this tomorrow, but I didn't think your BOM could include more than one configuration. Unless you are saying that your assembly included overlaying the same files on top of one another, but with different configurations.
        The BOM can have more than one config using the option to display configuration from same component as separate item.
        
        And in assembly, the files will be placed next to each other without any overlap.
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        Mattew Stafford @ Deepak Gupta on Feb 14, 2017 10:07 AM
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        Thanks! I think I just accomplished something similar to your suggestion. Where I first had an assembly (and corresponding print) with a part, I replaced that part with a subassembly. This subassembly included another subassembly that included (2) components (D5440 Panel 9), each with its own configuration. My BOM looks more like what I want now. Item 9.1.1 is one configuration of the weldment & 9.1.2 is the other configuration.
        Here is my "completed subassembly":
        And here is the sub assembly showing both configurations (blue highlighted is one config & the gray is the other):
        
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        Deepak Gupta @ Mattew Stafford on Feb 14, 2017 10:11 AM
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        Cool and yes that what I meant. You can also add exploded views in the assembly if needed.
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        Paul Risley @ Mattew Stafford on Feb 13, 2017 3:46 PM
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        Matt,
        
        Depak has good suggestions here for how to prep your next design, the dual weldments in 1 assembly is a way to go. When you do that I recommend lightweight and hidden on the 1 not being used a the main assembly.(ex if the welded frame is not for the assembly I would load it lightweight and hide it.) Lowers re-build time and grabbing issues that way.
        
        As far as configurations on your weldments that is an inherent function you learn over time. Build it to be configurable. 1 of the best time savers is linking plates / bar thicknesses to various configurations independently. We machine our plates after welding and we always give a control datum to where the first flat surface is, all other heights come from that surface. This gives us height controls versus the take .060-.080" to square up all plate surfaces.
        
        If configurations on your current weldment are limited by features there is the option to re-structure to get it where it is doable. Going forward though from this post and Deepak's advice you should have a good jump start on setting your next design to a configuration driven model that will yield you some pretty good results.
        
        Good luck.
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Trying to figure out sub-weldments

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