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Re: SE File Folder Structure

Experimenter
Experimenter

 

 


 

@RyanM wrote:

I am wondering what are your desired results? Your question is a bit vague and may be the reason we are not seeing many responses. Are there differences in your part numbers, CAD file names and drawing files? Does your design process or product start with a template and is then configured? Or is each product a unique product? Do you want to share data between products? Do you need part search and where used functionality, etc.

 

Here's my response base on what you have provided.

In my experience, the document of record for most CAD data files is a pdf. The pdf file is the document that is used and shared with the customers- both internal customers and external customers.

The CAD data and structure is used for many purposes but rarely as the document of record.

 

It has been well over 15 years since I have had to work in an environment that is still using folders and file locations. In the past, when a file is moved from one folder location to another the assembly files that the part is referened will fail to find it. This is true when you rename a file as well which you will be doing with your revision scheme.

 

You have the opportunity to look at your full process and determine what processes can be improved or automated. I'd highly advice this if you wish to get a "quicker" return on investment that you look at a bigger picture (i.e. Product Data Management PDM tools). These tools, when defined and implemented correctly, take care of the file management issues related to versions and revisions, file "locations", etc.


 

@RyanM We are moving from 2D AutoCAD, with drawings that have no associativity. I am trying to make sure that once we start making models and drafts that we don't run into roadblocks when we change filenames for revisions, move models, etc. as the assemblies, models and drafts all depend on linked files.

 

 

I will look into PDM, personally I think this would be our best option but I'm not sure that higher-ups will want to use that system, I've had a tough time even getting us to us 3D CAD thus far, they fear change. For our drawings/products we have a drawing no. such as 000-000-000-000-000 RA which is used to determine filenames, drawing numbers, and also call up parts in other assembly drawings.

 

Our drawing library and group aren't very big which is why I think that we might be able to get away without PDM. I've created templates for models, drafts, etc... is that what you mean? Or the basis of each product we make? Because we are somewhat diverse..... we do machining, fabricating, re-man of castings, large fabricated parts, mechanical buildings, etc. So each part is usually a unique part I would say. Some common parts are shared between product models as well have we have certain standard parts that are used in many products, ie. wall panels, doors, hinges, etc.

 

We do have a tendency (which I hate), of putting multiple assembly/maching/fabricating steps on a single drawing which tends to complicate things. I am trying to get us to move away from that practice, but I am certain that would give us some headaches if we try to retro-actively model/draft our existing products.

 


@bshand  wrote:

Sounds like a few of you guys should definitely consider PDM of some kind. Maybe just Insight. Trying to revise, release, and obsolete files while maintaining links to released files in active assemblies, etc. in an unmanaged environment is a nightmare. In my opinion and experience.

 

Also I agree that using PDFs to record releases is probably the best way. Making dumb editable drafts is much more difficult. And why would you want to edit released drawings anyway?

 

In a previous workplace (unmanaged) when a project was released the convention was to use revision manager to copy the whole model, even standard library parts, and all drafts to an appropriately named folder in which the files were zipped. It wasn't pretty and problems often ensued when these projects were copied out to use in new projects which were similar (a frequent practice) mostly having to do with duplicate file names which actually contained parts with differences than other projects so you never knew which was the correct one.


@bshand I guess that would make sense, once a drawing is rev'd up there shouldn't be any need to have anything more than a .pdf anyways.

 

How many people here use Insight? What other options are there? Is it included with ST7? We currently have 4 users in our office, and for the foreseeable future wouldn't have more than about 6. 

 

If we end up using an unmanaged system, I guess for revisions, we would probably save the old revision to the revision folder with a filename rev increment (ie, RB) but keep the current/new revision in the working folder, without a name change. So the filename wouldn't change until the revision is sent to the revision folder, and the assemblies will stay linked to the working file.

Re: SE File Folder Structure

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

Insight is included but you would likely need some support setting it up initially from your VAR or someone who has done it. And you would need a sequel server and the appropriate version of Sharepoint if you don't already have them. And you would need to appoint someone (preferably also well versed in Revision Manger use) as the manager of the Insight functionality for releases, etc. Some knowledge of Sharepoint is useful too but nothing extravagent is required.

I've been in unmanaged, Insight managed (currently) and Teamcenter managed environments. Teamcenter is overkill for most places. There is also SESP which is Insight on steroids. It has nice features but I don't know how wide a user base it has so wonder about its continued support. Then there are 3rd party solutions as well. Of the three Siemens solutions plain Insight is definitely the cheaper way to go.

Just my 2 cents and worth as much.

http://www.plm.automation.siemens.com/en_us/products/solid-edge/overview/insight_features.shtml

Bruce Shand
SE2019 MP5 - Insight - Win10 - K4200

Re: SE File Folder Structure

Phenom
Phenom

@MW_at_PD wrote:

 

 


 

 

@RyanM We are moving from 2D AutoCAD, with drawings that have no associativity. I am trying to make sure that once we start making models and drafts that we don't run into roadblocks when we change filenames for revisions, move models, etc. as the assemblies, models and drafts all depend on linked files.

 

 

I will look into PDM, personally I think this would be our best option but I'm not sure that higher-ups will want to use that system, I've had a tough time even getting us to us 3D CAD thus far, they fear change. For our drawings/products we have a drawing no. such as 000-000-000-000-000 RA which is used to determine filenames, drawing numbers, and also call up parts in other assembly drawings.

 

This is the kind of information we would need. Thank you for providing it. When moving from 2D to 3D management should habe been informed that you would need to seperate drawings from 3D models. This is know as the Master Model Concept.

 

Master Model Concept in its simpliest form allows for "concurrent engineering/design" and seperates and reduces the amount of data a workstation is required to open and load to view your 3D product. In these CAD environments (which is just about every 3D system out there) you get multiple files that represent your 3D product. Drawings are not exempt from this process- this is a change for your organizations since you are moving from 2D to 3D. Drawings reside in their own unique file (with the exception of Siemens PLM NX product- there are now changes in file extensions between a drawing, piece part or assembly all files are a .prt file). This concept applies to all levels of your product- from individual piece part to sub-assy/weldment to top level assembly. All have their own Master Model file and all other file types reference the 3D model file- its file name and file location! So here's a quick example:

12-30-2015 10-08-56 AM.png

This concept allows multiple users access the 3D model to complete their tasks and shorten the design time. As mentioned earlier this also removes the data associated with those tasks from the 3D model file making it a much smaller file and you don't have to worry about multiple people saving over files. Now this is for a single 3D model. Compound this for every 3D model you create and you will quickly understand why @bshand and I recommend a PDM system.

12-30-2015 10-17-40 AM.png

 

You do NOT want to be moving files around and making manual changes to file names or just opening one file and do a file-> save as. You can lose all those connections and make a mess really fast!


@MW_at_PD wrote:

 

Our drawing library and group aren't very big which is why I think that we might be able to get away without PDM. I've created templates for models, drafts, etc... is that what you mean? Or the basis of each product we make? Because we are somewhat diverse..... we do machining, fabricating, re-man of castings, large fabricated parts, mechanical buildings, etc. So each part is usually a unique part I would say. Some common parts are shared between product models as well have we have certain standard parts that are used in many products, ie. wall panels, doors, hinges, etc.

When I asked about templates I was thinking of configurable products- a product that adjust by making changes to specific design features like (L x W x H). It sounds like you do quite a range of different designs which have different design/engineering workflows and have different types of customer outputs. It still sounds like you need to setup a standard parts library which I believe you get with Solid Edge provides. Library files can be a different animal as well- Family of Parts vs individual files, etc. Others can assist you in those areas.


@MW_at_PD wrote:

 

We do have a tendency (which I hate), of putting multiple assembly/maching/fabricating steps on a single drawing which tends to complicate things. I am trying to get us to move away from that practice, but I am certain that would give us some headaches if we try to retro-actively model/draft our existing products.

 

 

Managing these types of processes are a challenge, as you now need to have a model for the casting/raw material for weldment and then the machined part/machined weldment. This should, in my opinion, require a dedicated process change.

 

An intitial analysis and system setup, of any new tool, will save you serious headaches down the line. If you haven't you need to sit down as a group and determine how your system should be setup to take advantage of the software and still provide ROI for your company! This will definetly require change on everyones behalf- because few 2D practices transfer to a 3D process. But I will conclude and congratulate you on your choice of software. You couldn't have picked a better toolset to help migrate from 2D to 3D! Seriously, Solid Edge provides you the best tools to aid you.

 

I just saw a posting by Russell Brook via Ken Grundey about another company that moved from 2D AutoCAD to 3D and Solid Edge. This might be an interesting read for you as well. http://ow.ly/MiRM2 The beginning is a little fluffy but get the middle and the meat of the article.

Re: SE File Folder Structure

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

I should say that the company where I work transitioned from Acad to SE 3 to 4 years ago. Insight was implimented shortly thereafter due to the wise direction of the engineering manager who "inspired" the move to 3D in the first place. The users were also new to 3D and to some extent are still adjusting to the relational aspects of solid modeling as well as some details with the software. I came here only about 1.5 years ago so am not intimately familiar with the early struggles. I think though that the early adoption of Insight may not have smoothed the 3D learning curve but I do think it forestalled future headaches with database management that we'd likely be dealing with now.

Bruce Shand
SE2019 MP5 - Insight - Win10 - K4200

Re: SE File Folder Structure

Experimenter
Experimenter

Thanks for the responses.

 

If I had an assembly, ie. 001-001 with a linked part say 001-002 and I were to save a part revision as 001-002 RA, the assembly is still linked to the original 001-002, correct? or is the assembly link updated when the part filename is saved-as?

 

On a lot of our products we bring in basic parts, such as rectangular plates, round bar, pipe, etc. Can you get these parts in adjustable dimensions in standards parts or can you create a library yourself?

Re: SE File Folder Structure

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

I haven't really used it as such but the save-as which saves in the assembly is weird in that it seems to only work once in an assembly. If I bring in another part it won't work again and the only option is save copy as. I usually usually use revision manager or save as copy then replace the old with the new.

As for various material shapes like structurals, tubing, bar and pipe we make a 12 inch long extrusion and save write protected in a standard network folder named accordingly and consider them templates. Then the user will open the template file, do a save as, and bring that in to the assembly.

There are shapes in the standard parts library but if I use it I only use it as a source for profiles.

Bruce Shand
SE2019 MP5 - Insight - Win10 - K4200