Data Management of SE 1

[MadMango]

I've been tasked with finding out exactly how well the built-in functions of SE are for data management and BOM control.

I am a long time (almost 6 years) user of SolidWorks, and I recognize several posting handles here from the SW forum. I am looking for real-world examples of how well SE out performs SW "out of the box." SW relies on 3rd party solution partners for most of their non-modeling functions. While this doesn't seem to be a bad tactic, there must be something good about the way SE has tried to intergrate BOM control and other things into the core package.

Visiting product sites you can't get a good idea of what a software is realy capable of, since they are all written with the "we're the best" slant. I want you guys to pour your manufacturing-ladden hearts out to me. Looking for any and all insights... "The attempt and not the deed confounds us."

 

[JamesBarlow]

I have used both the document control and BOM portions of SE with some good sucess. But, I have do have a few comments.

The revision control for documents is a little tedious to use. There a number of steps required to up the revision of a drawing, but it does work OK. Interms of actual control of the documents durring use I can't really say. I work with 3 other designers who who use SE, so the problem of different people working on the same drawing is something I have never had to deal with.

The BOM stuff is also pretty good. I have not gotten in to it very deeply, but for what we do I like it. It only takes a few clicks to create a bill on a drawing and flag each item. We have to manually transfer this information to our production and purchasing system (we use Excel for everything) so any changes need to made by hand. This gets a little much, but this has more to do with how we do things than the software.

If I had my choice, I would have purchased a third party document control package first thing. Most of the controls in SE, as well as most other packages, were added as an after thought to the development of the modeler. The third party stuff is from companies that only do document control. No matter how go the functions that come with the 3D software are, I don't think they will every really be as good as what you can get from other places.

I will also add that we are running SE V10. I know that this new Insight software from SE sounds pretty godd, but I have never actually used it.

 

[swertel]

WOW MadOrange, didn't try to narrow down this topic at all, did you? You got my head spinning.

First of all, SE is heavily dependant upon File Properties. More so than any other Windows based or M$ program that I know. The beautiful part is that for most of the file properties that are, let's say required, can be prefilled by the use of templates and standard data files. These standard data files, as I'm calling them, are text files (very easy to program) that can be stored on a network and pointed to by each specific user. They can also reside locally on some machines and pointed to there, depending on your need(s).

File control:
One of the tab in the file Properties dialogue box is Status: Available, In-Work, Review, Released, and Baselined. Basically, a brand new file is available to everyone. Once a designer begins working on it, he changes the status to in-work. This allows changes to the file by only the user that changed the status to in-work. It is available as read-only to everyone else. Once the file is complete and ready for production, the status is changes to release. This locks the file and can no longer be modified by anyone. In order to make changes to the file, you must rename the file (add a revision notation to the file name, for example). It then becomes available again for the cycle to repeat. Baseline is for purchased parts. They are modeled once and should never have to be changed again. Personally, my department does not use the status tab because we still consider the print document the master and therefore don't keep an electronic revision history. By doing so, we don't want to have to change the file name to keep a revision history.

Revisions / Link Management:
You are undoubtedly familiar with SolidWorks Explorer. SE has a program call Revision Manager which is just a SWX Explorer to the 10th degree. It is leagues ahead of SWX Explorer. Moving, renaming, copying, replacing files is a snap.

BOM:
SWX uses Excel to create the BOMS. SE has its own BOM creation tool that uses the data inside of the file properties to fill the fields. The upside, when you update the BOM, your added desicriptions are not removed as they are in SWX. The downside, you have to have all the fields you want in the BOM to be somewhere in the file properties. Typically they are located under the Custom tab. I remind you, though, that you can pre-fill tags in the Custom tab through templates and the standard data file. To save the data in the BOM to and outside program, such as Excel, is a simple right-click on the BOM. SE also creates reports, which are separate text files that can be of BOMS, Where-used, and several others.

New to v11:
Version 11 of SE adds a new program that is part of the core of SE called Insight. Insight is a PDM system based off of Microsoft SharePoint. It is completely transparent to the user. Insight is supposed to store all the files in a vault on the network drive. When a file is checked-out, Insight automatically caches a copy of the file on the local computer so all work is performed locally and not over the network. Insight will not utilize the network again until the file is checked back in. Insight is advertised as being bullet proof as far as tracking files and maintaining links. Since the investment for M$ SharePoint is rather involved, my company has not yet institued Insight so I cannot talk about it more than what I read on the SE newsgroups and get from other users.

--Scott

 

[MadMango]

Thanks for both of your replies. A few more questions for those that feel up to answering them...

How "customizable" is the SE BOM layout, as related to the number and length of "headings"?

Do you have the option to do Top-down or Bottom-up numbering, and can you break the BOM into parts (place 1/2 the BOM on one page, place the other 1/2 someplace else)?

How well does the BOM update? For example, if you have an assembly, and due to some redesign, eliminate 2 parts, and add 1 new one. Does the BOM number renumber correctly, or does it skip a beat?

Lastly (for this round anyway), has anyone out there tried to tie their BOM info from SE to their companies existing ERP/PDM systems? how easy or painful was that?

Thanks in advance. "The attempt and not the deed confounds us."

 

[swertel]

Prepare for another text book.
(By-the-way, you're lucky things are a little slow at work this week.)

The BOM layout is FULLY customizable. You can have as many headings as you want and you can control the width and text justification of each column. The headings are driven by the file properties of the part (assembly) of the view in which you selected to create the BOM. After placing the BOM, right-click and select properties. Click on the Columns tab. The Available Columns will appear which are properties in your part file. You can add any of these into the Columns Used and reorder these to appear the way you desire on the BOM. Select each heading in the Columns Used and change the Title Text, Title Alignment, Data Alignment, and Column Width.

The layout of the BOM is controlled by the standard data file Draftlist.txt. If you know what you're doing, you can just modify this text file. If you're like me, you create a dummy part that has all of the fields you want in the file properties. You then insert that part into a draft and create the BOM. Then select the BOM, right-click and select Properties, change all the settings you desire, and save the settings.

The Sorting tab of the BOM properties controls whether it is top-down or bottom up. A check box tells SE whether to create the list bottom to top (checked) or top to bottom (unchecked) Another tab control the placement of the BOM title block (headings): header, footer, both, or none. You split up the BOM by giving it a maximum height. Once it reaches that height, it creates another column spaced at a distance that you set in the BOM properties. You cannot place split the BOM up onto different sheets without loosing its associativity.

The BOM updates like any other drawing view. When changes are made to parts/assemblies that causes the BOM to go out-of-date, it will show up with a grey box around it. The BOM will update when you Update-all-views or when you right-click on the BOM and select Update Parts List. As far as renumbers, you are vague in your desires. I'll go through three examples.

(1) SE BOM setting is set to renumber items.
If you delete two and add one part with this setting checked, lets say deleted items 2 and 3 and have a total of 6 items. The new part you added will become item 2. The remaining items vary in results. The last item, 6, may become item 3 and all the other items will remain the same; or all the items will be renumbered to one item lower, 4 to 3, 5 to 4, 6 to 5.
(2) SE BOM setting is set to NOT renumber items.
If you delete two and add one part with this setting checked, lets say deleted items 2 and 3 and have a total of 6 items. All item numbers will remain the same. The new part will be item 7. The numbering in the BOM will not be sequential, it will be 1, 4, 5, 6, 7.
(3) When we delete items, we need to show DELETED in the parts list. We can't just non-sequential numbers or gaps in the numbering scheme. So, we ground the part in the assembly, we modify the part to delete all the solids, and modify the part description to say DELETED with a quantity of -.

Lastly, don't have one. Never tried.

--Scott
P.S. Took too long to write. Didn't spend any time proofing.