Hi,
I created this weldment part using Solid Works
2016 sp2.0, and I have problem relate the duplicate balloons, please I would
like to know if there is a method that I could control this but in parametrical
way, a settings something relate the cut list table, similar with the settings
from assembly and BOM table where we could control the balloons duplicate,
thank you I really appreciate. Please see the ppt from attach. Best.
Sorin,
Always better to upload the model and drawing than a powerpoint that cannot be analyzed (for me anyways because I have not used cut list tables since SW2012; now use indented Bill of Materials table). Anyway do you have your views linked to the cutlist bom? Cut lists can only be created from as welded configuration unless you have deleted this config. Are your views of the as welded or as machined config? Are there differences between the as welded and as machined configurations?
I use Default As Machined like configuration, So I didn't delete any configuration. Relate the solid works files, I cannot provide from confidentiality reason. So usually in weldment environment I use all the time cut list table and not BOM, from assembly, and I would like to remain like that. From the ppt file, it is easy to read and from the cut list table and from the 3D view the same that balloons 9 with 1, 7 with 2, and 8 with 5, where appear this duplicate. Thank you for your answer, I appreciate.
Best,
Sorin,
Cut list tables are ok if they work for you. Looking at you PPT only it appears item 1 has pad 6 welded onto it. Does the hole in item 6 go into item 1. If so then 9 and 1 and not the same. Also depending on how you modeled part the hole could be breaking into item 1 (just cutting the surface) so SolidWorks thinks item 1 is different). Items 2 and 7 appear to me to be opposite hands so they would not be grouped together. Again without model, items 5 & 8 are too small to determine if there are any differences. Are 5 & 8 modeled the same way, I have seen parts that were modeled differently to same size that SolidWorks treats as separate items.
If you cannot provide model due to confidential reasons, can you save it out as a parasolid and provide that. Just looking at the bodies can sometimes help diagnosis the issue. In fact you could do the same, open the parasolid, add a weldment feature and see how the bodies get grouped.
Thanks, I appreciate. So is clear if the members are created in different group even are the same angle type length material weldment read like different, ok but what about the plates 5 and 8 are only simple extrude plates with the same dimensions size etc, etc... thank you, I appreciate.
Best,
Sorin,
Dimension the plates out to 8 places including the hole location and size to see if there are any differences. I also asked how these parts are modeled. Are they modeled the same way? Patterned? Mirrored?
If you want to combine those items, you do know that you can drag the bodies into different cut list item folders?
I would like to atach a step file of this weldment but I didn't find the atach file options on this replay window thanks, I appreciate. The plates are simple extrude with sketch in weldment module, because the geometry reference old dwg consideration I used this method, thanks. Sorin,
Parasolid would be better than step. Below is how to attach file.
Edit: Screen shot of your feature manager tree would also be helpful.
Check #18 of Forum Posting on how to attach files while replying to a post.
Thanks, I very appreciate.
Thanks for hint. The button for attach didn't appear near Mention...
Best,
Sorin,
Thank you for the parasolid; answered many questions. Items 1 & 9 the 0.5625 diameter holes in item 1. For items 2 & 7 they are opposite hands. For items 5 & 8 even though they are the same length, width and thickness the 0.5625 diameter holes are in different locations by 0.00034641. Granted not much but enough for SolidWorks to see them as different items. If those holes are put in after the items are welded then the holes should be suppressed in the <As Welde> configuration and the bodies will most likely combine the way you want them to. I hope this helps.
thanks, I appreciate very much, Solid Works is become interesting.
Best,
Sorin,
Thank you for the parasolid; answered many questions. Items 1 & 9 the 0.5625 diameter holes in item 1. For items 2 & 7 they are opposite hands. For items 5 & 8 even though they are the same length, width and thickness the 0.5625 diameter holes are in different locations by 0.00034641. Granted not much but enough for SolidWorks to see them as different items. If those holes are put in after the items are welded then the holes should be suppressed in the <As Welde> configuration and the bodies will most likely combine the way you want them to. I hope this helps.