In assembly drawing which contains some views, I replaced the Assembly model, in all views.
? How can I update the BOM to show the new model items
I'm pretty sure you can't. You will need to delete that BOM and insert a new one.
Although you need to have a drawing view active to insert a BOM, the BOM is then linked to the assembly itself, not the drawing view, so there is no way to update an existing BOM to reflect a new drawing view.
I think I should open Enhancement Request for this issue.
You can certainly do that if you want, but I don't think it's that much trouble to delete a BOM and re-insert it. If you do submit the request, please don't ask to change the way BOM's are linked now. Maybe ask for something like a right-click option on BOM's to change the reference. I personally wouldn't want BOM's linked to the drawing view instead of the model. I sometimes have a BOM that takes up a whole sheet, and it's nice to be able to delete the drawing view after inserting the BOM to get it out of the way.
Yes it is a lot of trouble, especially when I have modified the BOM table format (i.e. set and locked column widths, etc.) If I can replace the model in a drawing, I also should be able to point the BOM to the new model reference and not have to delete and re-insert the BOM.
As I understand the purpose of replacing the model in a drawing file, it is so the FORMAT of the sheet can stay the same. Having the BOM reference an assembly that is no longer shown in the drawing seems like either a bug or a glaring oversight.
If you have the table adjusted the way you want, you should be able to save it as a BOM template and use it when inserting the new BOM.
If you lock your column width and you would add a new component that has an extra long part number or description, how does your BOM change?
The text wraps and the row height changes.
Regardless, the argument that deleting and re-inserting the BOM after model replacement is an acceptable workflow is invalid, especially because when the model is replaced by changing the file reference when opening the drawing file, the BOM and other tables update to the new model reference with no problems.
Why does it NOT do this if the model is replaced using Tools>Replace Model...? This certainly appears to be a bug, a flaw in the programming, an oversight, call it what you will.
Without updating the tables to reference the new model when replacing the model in the drawing file, the Tools>Replace Model... function is useless.
The Tools>Replace Model command is not entirely useless, as that is the only way to change the model reference in a drawing file from a part to an assembly. You cannot replace a part with an assembly by changing the file reference before opening the drawing.
Yes. It is possible. But is tricky.
The procedure for the creation of the new drawing has to be different. The replace model method does not update BOM (or baloons).
PRELIMINARY NOTE: IF YOU HAVE WRITING ACCESS TO THE ORIGINAL FILE I STRONGLY SUGGEST YOU TO MAKE A BACKUP COPY OF IT IN CASE YOU MISSCKICK SOMEWHERE.
I USE READ ONLY MODE IN THE ORIGINAL DRAFT I WANT TO MAKE COPIES OF, THEREFORE THERE ARE NO MISSCLICK RISKS.
In practice, one has to:
1) file, "Open..."
2) in the window Open, select (without open yet) the original file you want to make a copy of.
3) In that same window (Open), click the tab button (bottom right for me but may depend on version) label "References..."
4) the window "Edit Referenced File Locations" is open, double click on the original reference ("name" column, not the "In Folder" one)
5) a second "Open" window is open and now you must select the new model you want to make the new drawing and click Open
6) you are back in the "Edit Referenced File Locations" window where now the reference of the original draft have changed. click "ok" to close window
7) you are back in the first "Open" window with the original draft selected, click Open now.
8) Go to file "Save As..." and save a copy of the draft with the new name and location. Voilà.
The new draft has BOM updated to the new model and so do the views and baloons.
PS: I apologize if there are any typing gaps but the window keeps bouncing on top of the page every time i press a key, so in practice I write without looking what I'm writing because the post is in the bottom of the page...
PS2: I use SolidWorks 2016 and Windows 7
Probably reinserting BOM is the simplest way to deal with as been shown by Glenn Schroeder earlier in this thread.
Probably for you Vladimir Urazhdinbut I did give the actual Answer to the Original Rafi Sokolquestion.
Another possibility is to do the drawing all over again. lol
But the point of keeping the original bom might be handy when it list 150 components that must keep a "user defined" order instead of a random one. Plus the reinsertion of 150 baloons.
An 8 step procedure for ACTUALLY DOING WHAT IS ASKED is not such a complication.
Each user might have its own personal motivations to do a thing in a specific way...
I see this thread is pretty ancient but it's an issue I have simply tolerated for a while and if there is a remedy I would surely like to find it...
Glenn Schroeder, I tend to agree with Scott Moore on this one. I use SW to write shop assembly instructions, so in my drawings the BOM's are more of a components list for the assembly techs to reference. I typically include a column on the right for assembly notes that pertain to particular components. These notes tend to change and do not fit the template idea. They are however, associated with the row of the particular component. If my 'BOM/component list' would update to the model currently being referenced by the drawing it would save me a lot of time & effort.
That last sentence above brings up other interesting points.
I have currently arrived at this conundrum via Pack-N-Go, but I have tried numerous work-flows to copy a project (Windows copy-paste-rename-replace ref's, SW Explorer...etc., etc.) including similar to the one described below by Pablo Peraffan. They all have their issues as far as I can tell...and none seem to have any positive effect on what is being discussed here..
So is this just how it is for SW users? I have been doing exactly as Glenn suggests, recreating BOM's, notes & all, page by page...
With ten or more BOM's in some drawings it is very time consuming..
If someone knows of a quicker/easier method please share!!
James Harvey wrote: Hey guys,I see this thread is pretty ancient but it's an issue I have simply tolerated for a while and if there is a remedy I would surely like to find it... Glenn Schroeder, I tend to agree with Scott Moore on this one. I use SW to write shop assembly instructions, so in my drawings the BOM's are more of a components list for the assembly techs to reference. I typically include a column on the right for assembly notes that pertain to particular components. These notes tend to change and do not fit the template idea. They are however, associated with the row of the particular component. If my 'BOM/component list' would update to the model currently being referenced by the drawing it would save me a lot of time & effort. That last sentence above brings up other interesting points.How is it that this drawing BOM is referencing an entirely different assembly than that which is in the drawing views, yet when I go to 'File>Find References...', SW only lists the models I currently have in my drawing?When I look in my Bill of Materials property manager under Configurations- it indicates that it is referencing the correct model, so WTF? (FYI: When I reuse an assembly, I revise the filename (of course!), configuration name & descriptions of the top level assy and of several sub-assy's within it...it is these sub-assy's in my BOM that are retaining the old part number & description from the assy which they were derived). I have currently arrived at this conundrum via Pack-N-Go, but I have tried numerous work-flows to copy a project (Windows copy-paste-rename-replace ref's, SW Explorer...etc., etc.) including similar to the one described below by Pablo Peraffan. They all have their issues as far as I can tell...and none seem to have any positive effect on what is being discussed here.. So is this just how it is for SW users? I have been doing exactly as Glenn suggests, recreating BOM's, notes & all, page by page...With ten or more BOM's in some drawings it is very time consuming.. If someone knows of a quicker/easier method please share!! SW2017 SP3.0Windows 7 Best,James
James Harvey wrote:
That last sentence above brings up other interesting points.
Instead of writing the notes directly in the BOM, assign a custom property at the Part level for them, enter the information there, and add a column in your BOM template that references that property.
Sure you can enjoy to proceed with 8-th steps process and waste your time (not sure if your time is valuable enough for your company), but I’m still believe that the two clicks procedure (delete old BOM, insert a new one) is much simpler and faster. Unless the old BOM contains unlinked items like additional notes, fake part numbers, materials, etc.
That's a great idea Glenn, for me 2 problems arise:
1) I have had problems with custom properties cooperating as expected, my own fault, I need to practice/experiment more with them (and I admit it's been a while...)
2) Due to space constraints the note column often has text that says, "note 1" etc. referring to a list of notes elsewhere on the sheet. These frequently change dependent on the project.
I'm sure there is a way to make all of this somewhat automated. Taking the time away from the daily grind to accomplish it is another challenge altogether...
Thanks for the input always!
Do you even read before Reply?
Reinserting a BOM makes default item numbers. My company does not use some random default SW numbering. Every component has to be in a SPECIFIC position in the BOM. And also reinserting BOM implies reinserting baloons because also baloons have the same reference issue as the deleted BOM.
Maybe I am missing something but the only way I know to change item position in the BOM is via drag and drop THAT TAKES WAY TOO MUCH TIME WHEN DEALING WHITH HUGE ASSEMBIES. Sum up the New baloon insert and positioning and it is WAY MUCH more than the 20 seconds required by the method I described before.
Vladimir Urazhdin If you want to keep trolling and makig fun of me, my time, my company and clinching your "do all over again" technique please just save your precious time instead. You don't need the method? For you is ok to do it all over again? We all got it.
If you know a quicker way to to assign the BOM position number to a specific component, reply. Otherhise you are just trolling or in the wrong post.
Maybe the fact I put too many details into the procedure makes it seem more difficult that it actually is. some steps take milliseconds and the overall time is of about 20 seconds mainly due to model loading time. Try to replace references before saving the new file. It will replace all model references properly.
Just my curiosity.... What in the reason to keep part numbers / positions unchanged if some assembly items have been replaced?
Third party BOM management APPS for example, to which SW must match.
Each user may have it's own reasons. But we dont discuss reasons. Here we discuss SW procedures to achieve specific requests...
The method I posted matches the specific request posted in this thread. If one need it or not is offtopic.
How about this?
Open drawing you want to replace with new assembly model.
Open assembly model currently referenced by drawing.
File, SaveAs assembly model to file name of new assembly model to be referenced in drawing (not in same folder as new assembly).
File, SaveAs drawing to new name.
Close both drawing and assembly.
Open new assembly model.
Open drawing saved with new name.
Select "Accept this file anyway" in the dialog that pops up.
There may be other dialogs that display, answer appropriately.
BOM should now be looking at new assembly. Only quirk I found is that configuration name in old and new assembly models should be the same name that the BOM is looking at.
I know this is a lot of steps again but at least the BOM does not need to be replaced.
I just had the same problem and spent too much time trying to solve it. It didn't make sense that all of my views are the new assembly but the BOM is still referencing the old. Even in FILE/FIND REFERENCES, still showed I was looking at the old and new assembly. I gave up on trying to salvage the old BOM and inserted a new one. I inserted the new BOM and picked the same view without deleting the old BOM and no good, it was the same thing. On a hunch inserted again and I chose a different view when inserting the table, still without deleting the old BOM. This worked, the new BOM correctly referenced the new assembly. I formatted as needed and deleted the old BOM. Checked the file references and now only the new assembly showed up. Just for a test, I inserted another BOM and chose the original drawing view that my first BOM was linked to and it also showed the new assembly.
Bottom line, it seems that if you are having trouble with table references you need to delete it and recreate.
Bogus, Solid Edge has no problem with this... well, it works most of the time.
This process is easy and worked great for me. Already had the new assembly created and kept the new drawing the same with boms and balloons, much easier for the shop floor and documentation having similar drawings. Thanks!
If the new assy has the same file name, the 2D drawing accepts the new geometry but the dimension does not (new geometry it's too different)
Some time ago I made it to make new pressure vessels using the same basic geometry
LOL you need to lower your expectations. SW is not like other software in 2018, where you can just count on it to get better, more functional, and easier over time. Nor is it like software in 2008, where you can count on it to crib useful features from other programs and give the user easy transitions between packages.
Think of SW like a time traveler from 1988. The software is your adversary and you must "beat" it. That means giving it as little control as possible over your work and avoiding ALL "automated" activity (which are traps).
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