23 Replies Latest reply on Sep 23, 2014 4:57 PM by Chris Scheer

    Weldment BOM

    Chris Scheer

      I have a single part which contains a weldment frame structure (Multiple frame pieces).  When I bring it into a drawing, and try to create a BOM, it creates a single line item treating the part as one part.

      To create a BOM of this weldment structure, do all individual frame pieces need to be individual parts or can I keep the whole frame structure in one part on the drawing and have a BOM identify each individual pieces?

       

      Thanks

        • Re: Weldment BOM
          Daniel Andersson

          Have you tried using a cut list instead of a bom?

           

          You should be ok with cut list. If you keep each item as separate body and have the weldment feature in the feature tree.

            • Re: Weldment BOM
              Chris Scheer

              How do insert a cut list?  Where would I find it?

                • Re: Weldment BOM
                  Michael Sutherland

                  Under annotation tab there is a button called tables that expands.  You will find cut list table there.

                    • Re: Weldment BOM
                      Chris Scheer

                      Hmmm.. I only see have these in the pull down menu...

                      cut list.jpg

                          • Re: Weldment BOM
                            Chris Scheer

                            As you can see, the Weldment cut list isn't an option for me, but I think I know why...

                             

                            When I create a drawing from my original multi-body part (which includes my weldment frame work, which I created there), it shows a cut-list in the feature tree, and allows me to create a cut list in the drawing.

                             

                            When I create a drawing from the frame part (which I "saved out" of the original multi-body part), there is no cut list in the tree... it appears "Solid Bodies" has replaced it.

                            Therefore, I'm unable to create a cut-list in the drawing with my frame part by itself.

                             

                            I guess the solution is to create my drawing from the multi-body part.. But that's what I was trying to avoid.  I'm still new with solidworks, and was trying to keep it simple with my framing... so JUST my framing is in the drawing...

                             

                            I think Daniel might have touched on this.. When he said "as long as my weldment is in the feature tree"..

                            Weldment Cut List.jpg

                              • Re: Weldment BOM
                                Glenn Schroeder

                                Can you explain your workflow a little more? Especially why you're reluctant to use the original part in your drawing?  I create drawings of multi-body parts all the time, with cut lists, and don't have any problems with it.

                                  • Re: Weldment BOM
                                    Chris Scheer

                                    Hi Glenn,

                                     

                                    I'm still trying to establish my work flow.. What's going to work best for me.

                                    I went ahead and used my multi-body part in a drawing, and it seems to be working well.  Few questions on my cut list (see image).

                                     

                                    1) Any idea why some items (like 1 - 4) have such a long, drawn out description, and other items (like 6) are more simple, less information?  (I like the way item 6 is identified).

                                     

                                    2) Is there a way to have non-structural memebers be a part of my weldment cut list? (Ex.. Item 5 is a 8x8 x1/4" base plate that is currently left blank in the cut list.

                                     

                                    3) Some item numbers in my cut list don't exist and are blank (9, 10, 12, 13, 16, 22-68).  Are these items in my multi-body part that aren't showing because I didn't select them using "select bodies"?  If so, can I get my cut list to only show what I'm showing?

                                    Frame Cut List.jpg

                                      • Re: Weldment BOM
                                        Glenn Schroeder

                                        Chris Scheer wrote:

                                         

                                        Hi Glenn,

                                         

                                        1) Any idea why some items (like 1 - 4) have such a long, drawn out description, and other items (like 6) are more simple, less information?  (I like the way item 6 is identified).

                                         

                                        Those Descriptions are probably coming from the .sldlfp file, and it appears there are links to dimensions in that file that have gotten lost.

                                         

                                        2) Is there a way to have non-structural memebers be a part of my weldment cut list? (Ex.. Item 5 is a 8x8 x1/4" base plate that is currently left blank in the cut list.

                                         

                                        Yes.  Expand the cut list at the top of your tree, RMB on the body name, and choose Properties.  You can insert properties there just like you would for any other custom property.  Including having dimensions visible and linking them to the property so they're parametric.  However, for the future, if you'll be using weldments fairly often, I'd recommend creating .sldlfp files of Plate, with the Descriptions linked to the plate dimensions, so you don't have to do all that manually.

                                         

                                        3) Some item numbers in my cut list don't exist and are blank (9, 10, 12, 13, 16, 22-68).  Are these items in my multi-body part that aren't showing because I didn't select them using "select bodies"?  If so, can I get my cut list to only show what I'm showing?

                                         

                                        It's hard to say what happened there without seeing the file.  Right-clicking on the Cut List folder at the top of the part's RM tree and choosing "Update" from the drop-down might fix it.  If not, you can always expand the cut list folder, RMB on a body, and choose "Exclude from cut list".

                                         

                                          • Re: Weldment BOM
                                            Chris Scheer

                                            Glenn,

                                             

                                            Thanks.

                                            1) You were correct about the .sldlfp file.  It was one I tried to create on my own, but didn't do it right I guess.  I've since "saved as" an already created profile, adjusted the dimensions accordingly.

                                             

                                            3) You were also correct about needing an "Update"

                                             

                                            2) This is where I'm having trouble.  I see how you can insert properties, but I've never created custom properties yet, so having some "language" issues... I can't get the "Evaluated Value" to display what I want.  I'm also having trouble creating a new .sldlfp file for the plate, as I haven't done that yet, either.  I will need to study.'

                                             

                                            Thanks.

                                              • Re: Weldment BOM
                                                Glenn Schroeder

                                                Here is one of my files for Plate.  Put it in your folder location, and you can Save as.. for other sizes.  The dimensions will update for the custom property.  I have it set as "TYPE", but you can change it to Description easy enough.  Just go to File > Properties, then select "Description" from the drop-down in the Property Name column.  By the way, I don't try to have one for every size.  It wouldn't be possible anyway.  When I'm using one of them, if it's not the right size, I just use one that's close.  Then after closing out the Structural Shape function I expand it in the tree and edit the imported sketch to the desired dimensions.  Since this sketch is only copied over from the .sldlfp file I can make changes to it in the part without affecting the original file.  And since the custom property is linked to the dimensions, the cut list property will reflect the accurate dimensions.

                                                 

                                                As far as getting the "Evaluated Value" to display correctly, just enter what you want in the "Value/Text Expression" column.  If you want to link to a dimension, then have the dimensions showing in the graphics area, and click on one when your cursor is in the correct place in the "Value/Text Expression" column.

                                                 

                                                Feel free to come back with more questions if you need more information, or a better explanation.

                                            • Re: Weldment BOM
                                              John Porter

                                              Hi Chris,

                                               

                                              It appears that your weldment does not have the imbedded "Cut List" between Annotations, and Material in the feature tree...It would be difficult for a Cut List Table to populate if the Weldment Cut List in the feature tree does not exist.  This could be an issue.  I would just create a new part, and start over importing the 3d-sketch from your existing weldment, and see if it creates a cutlist automatically like it should...if not you have potentially bigger issues.

                                               

                                              Our workflow for Skids for example:

                                               

                                              1) Create the actual skid layout (Beams, cross beams, welded sole plates, and lug plates) A welement should create a "Cut List" between Annotations, and Material in the feature tree that you can select and selecting "update".

                                               

                                              2) Create the Checkerplate deck on the Top Of Steel "in context" so if the size changes the checkplate updates

                                               

                                              3) Create a new assembly and drop the skid weldment into it, constrain appropriately

                                               

                                              4) add all extras (bolted lifting lugs/parts, hardware, loose items)

                                               

                                              5) Creat drawing of assembly

                                               

                                              6) Insert a BOM, select "indented", use "flat numbering", select "detailed cut list", under "Part Configuration Grouping" select "Display Configurations of same part as separate items", and all items will appear on the BOM as individual bodies, including all weldment bodies.

                                               

                                              Just some thoughts...I hope they help.

                                                • Re: Weldment BOM
                                                  Michael Sutherland

                                                  Hello John, maybe you can resolve some questions I have on approach and workflow. My company does a lot of steel structures and i would like to use weldments but run into a problem because we use bolted connections. So we have connection plates welded to the ends of beams and the beams have holes for cross supports and such. Each beam requires its own drawing even if they are the same length the hole pattern typically differs. Could you explain to me how you would approach this? Im thining of using weldments but as far as the plates would I insert as part or weldment profile and trim? Then save as multibody? I would also like to keep it as parametric as possible. Thanks in advance.

                                                    • Re: Weldment BOM
                                                      John Porter

                                                      Hi Michael,

                                                       

                                                      We would model the weldment structure complete as you can get it, then:

                                                      -drop it into the frame assembly (there you can drop several weldment structures, your connection plates, and any other loose items (fasteners, etc.)

                                                      -edit the weldment in-place, create a sketch, and project the hole pattern for the connection plate onto the beam, and cut the holes (in-context). Do this for all the places you have connection plates.

                                                      -now that the holes are in the weldment structure elements you need to detail them individually in the drawing

                                                      -in the drawing, make sure the weldment with the beam you want to detail is open in another window, select "relative view" from "view layout," tab,  select the "Window" tab from the top bar, and select the weldment.sldprt window with the beam, check "selected bodies", then select the beam, select the front face, sleect the top face(or whichever ones you wish), and drop it into the drawing.

                                                      -scale, label, detail, create top, end views, and dimension as you normally would.

                                                       

                                                      this works great for us...took a little to get that to work right, but it works great for our skids/structures.

                                                       

                                                      LMK if this helps.

                                                        • Re: Weldment BOM
                                                          Michael Sutherland

                                                          I think that will do the trick. As far as modifying the structure for another job would I change the dimensions in the original weldment? Would the plates inserted in the frame assembly move accordingly? And if only certain beams changed would there be a way for me to know so I could assign it a new part number and keep the other unmodified pieces without giving all new part numbers? Sorry if I seem like an endless bucket of questions, im the only person at my job that has any experience with Solidworks but don't have much experience with its application to manufacturing. Of course it falls on me to figure it out, everyone thinks its magic and does everything you need with a touch of a button.

                                                            • Re: Weldment BOM
                                                              John Porter

                                                              Michael,

                                                               

                                                              I know exactly what you mean.  I always refer to the Star Trek IV movie when they go to the past, and Mr. Scott starts speaking commands to the computer.  It is pointed out to use the mouse, he picks it up and says, "Computer....Make it so"...yeah...everyone that doesn't use it thinks Solidworks is that easy! 

                                                               

                                                              Basically you have to think about how your structure could possibly change...grow in width, height, etc.  then constrain the parts/subassemblies with some kind of logic that could keep them without blowing up if the subassemblies are modified.  Sometimes...Ok...most times...it is really hard to predict the off-the-wall requests to modify something in a way that makes no sense...but it happens.  A little planning goes a LONG way to helping with that situation.

                                                               

                                                              For you, I would start the structural assembly with the one weldment structure(the one that "should" never move), constrain it completely. Use that as you ONE anchor point, and build off that. use you connection plates to place the other weldments.  If you build it in Solidworks the way it would be built in "real life" on-site, you have a much better chance of being able to deal with future changes. 

                                                               

                                                              With piping skids, we lock down the pump as our "anchor" in a "pump train" sub-assembly. we then build the piping one gasket, spool, valve, and meter at a time. When the pump train subassembly is done we drop it into a "piping assembly" sub-assembly with all the other "pump train" subassemblies.  We then drop the "piping assembly" subassembly into the General Assembly, with 3 constraints, with the skid, building, stands, heaters, loose equipment(each having 3 constraints).  That way, to move the entire piping assemly up or down is one value.  If an individual pump train has to move, you go into the pipe assembly, and modifythe 3 constraints holding within the pipe assembly. Think LEGO

                                                               

                                                              It's all in how you build the model, the logic of your part, sub-assembly, assembly strategy/workflow.  If a part has to move with another assembly, it should probably be constrained to the moving assembly, and not rigid in space.

                                                               

                                                              I don't know if I answered your question...I kinda rambled.

                                                               

                                                              LMK if you have questions.

                                                        • Re: Weldment BOM
                                                          Chris Scheer

                                                          Thanks John,

                                                           

                                                          I tried your "workflow" as a test with one of our products.  It seems to work well.  One problem for me, though, is isolating items in certain views in the drawings.

                                                          Our planset drawing would/will typically consist of a framing tab, some hopper tabs, wall tabs, etc.  In each of these individual tabs/views, I want to isolate ONLY the relavent item.  It seems in a drawing (created from an assembly) the only way to isolate certain items is to use the "Hide/Show Bodies" "Hide/Show Components".. That can take a very, very long time to select every item I don't want to see as we have a lot of components/parts in our assemblies.. Is there a better way?

                                                            • Re: Weldment BOM
                                                              John Porter

                                                              Hey Chris,

                                                               

                                                              See my reply to Michael above...I think it answers the question.

                                                               

                                                              If not...LMK

                                                                • Re: Weldment BOM
                                                                  Chris Scheer

                                                                  John,  I'm not sure if this is exactly what you were telling Michael to do, but here's what I just discovered, and it works GREAT for what I was trying to do...

                                                                   

                                                                  - Create drawing from my multi-body Assembly

                                                                   

                                                                  - Insert a view

                                                                   

                                                                  - Select "Model View" while in the "View Layout" tab

                                                                   

                                                                  - Pick a frame piece, drag it over.. It creates a view of the entire frame.  I also tried it with other parts.. I picked a wall, drug it over.. It created a view of all my walls. Perfect.

                                                                   

                                                                  - To select a single frame piece (or wall, or any component).. Pick your Frame view, select "Select Bodies", and you're able to select a single frame piece for detailing. Fantastic.

                                                                    • Re: Weldment BOM
                                                                      John Porter

                                                                      Hey Chris,

                                                                       

                                                                      Like everything with Solidworks, there is more than one way to the same thing.  Some work better is some situations, and others work better in others.  That's why I like trying different things, and different ways to do things in Solidworks.  You know what they say, "sometimes you discover the most amazing places when you get lost" Well...I've been lost an aweful lot with Solidworks over the years. 

                                                                       

                                                                      That was what I was telling Michael about, but it sounds like you discovered a slightly different way to do the same thing.   Nice!

                                                                       

                                                                      JP

                                                                  • Re: Weldment BOM
                                                                    Cody Zorn

                                                                    Chris,

                                                                     

                                                                    You could also select a certain body or bodies to show in a drawing view.

                                                                     

                                                                    Select the view which you want to show only certain bodies in, then click "select bodies..." in the property manager.  It will open the reference weldment for you to select the bodies to show.

                                                                     

                                                                    Weldments can be very helpful but also take a while to setup with library features, properties etc.  I would suggest reading as much as you can in the SW Help and watching either Youtube or your VAR videos before you go to far in the wrong direction.

                                                                     

                                                                    Use sheet metal features instead of boss extrudes to create your plate/sheet parts.  They include a lot more useful properties.

                                                                     

                                                                    Hope this helps,

                                                                    Cody

                                                                      • Re: Weldment BOM
                                                                        Chris Scheer

                                                                        Cody,

                                                                         

                                                                        That's funny.. I just posted about what you just told me about "select bodies".

                                                                         

                                                                        And using sheet metal features instead of boss extrudes to create plate/sheet parts sounds like something I should consider..

                                                                         

                                                                        Thx