checklist or set of company standards for making models 7

[duk748]

hello - our company has been going thru hell w/ solidworks ever since we had someone who knew nothing about setting up a solidworks users group to get our engineering group started in 3d cad - the person our so called expert just dumped the software in the engineers laps and said go for it - now we have parts & models w/ sketches under defined, planes & origins all over the map, etc. - does anyone have a set of standards or a checklist that their engineering group follows & is policed by in creating their models such as sketches must be all black, dims & datums on the models so they follow to the drawing , etc. - any help or documents that i could use as a boiler plate to follow for our group would be greatly appreciated - thank you in advance

 

[TheTick]

All sketches must be all black unless they don't need to be. (Good luck doing this if you change your sketch color to green.)

Model dimensions must follow drawing dimensions in all cases except where maybe they shouldn't.

All origins must be at coordinates (0, 0. 0). Planes must've on the map. The map must be flat. No globes.

 

[Jboggs]

Start with standardized document templates that include all the settings you want to commonize. Put them in a single location all users have access to. Solidworks installs all of the support files on the local drive unless you direct it otherwise. Move all support files to a single commonly accessible server location. Set the File Locations on one machine to access those locations. Set all the other settings on that machine to whatever standard you want. Then learn to use the Copy Settings Wizard to migrate those same settings to all other users. Once that is done then at least all new work will start from the same source.

Can you convince your company to invest in some on-site training? That's the best way to get everyone in the same room and establish a set of "Best Practices", like "all sketches must be fully defined", or "use mid-plane extrusions over blind extrusions whenever possible", or "learn to use offset extrusions rather than creating new planes", or many others. You have a long hard road in front of you, but if you can at least get everyone on board as to the value of a set of common best practices you can create your own. If on-site training isn't available, try to assign (or evolve) one or two "master users" that can serve to answer questions and slowly migrate those best practices among the group. Weekly departmental gatherings for this purpose can be very valuable too.

 

[TheTick]

A good way to start might be to have everyone check each others' work (or even take it over) and see what it's like to work on someone else's stuff.

 

[DiegoLGraves]

I usually don't mind working on models from customers because working them over to use for production is part of our service. But it is aggravating to work on a coworkers models when they've been using the software for 5 or 6 years and still are too lazy to do any more than get it off their desk. And then find out when they're on vacation that things I need to work on are only saved on their local drive, rant, rant, rant.

I second Jboggs recommendation to set up standard templates in a common location, and to use the settings wizard to get everyone looking at the same location to start with. Also standardize the design library with annotations, parts, forming tools, etc. We've beefed up our peer review process in the last couple years so at least non-standardized prints are easier to find before they leave the department. Our peer review check sheet is at a higher level than the sketches, generally it verifies the drawing is complete in a standardized format, and the routings are correct and complete. It's far short of a design review.

Good luck, it's worth the effort to pursue. Diego

 

[ctopher]

I suggest training.
Also, if you know the models are being created wrong, start your own in-house training once a week.
I do it now.

There are also ASME/ANSI/ISO/etc specs to follow that help.

Chris, CSWA
SolidWorks 14
ctopher's home
SolidWorks Legion

 

[SBaugh]

I am currently working on Contract to Perm (over a 6-8 month period) to write standards Document (drawing and modeling best practices) per their processes. I am also here to help them with training in Solidworks, settings up templates, and helping them find ways to be more efficient between Solidworks and EPDM. This process is not going to be a 1 or 2 month project its a several month project. Hopefully your management is willing to work with you or who ever is tasked with making this work. I am considering going into business for myself to do exactly what your looking for at your company. Problem is, I need to be onsite and these projects take such a long time... let me know if you need any help like that... but to answer your question you should look for:

1) SW Training from you VAR

a. Look at Solid Professor or I.Get.IT as an alternative​

2) Read / Search posts for questions you might have - I think of it like this when I hit a wall " I cannot be the only person that is having that issue?"
3) Search Solidworks World presentations or VAR websites. 3DVision posts their presentations from all those that presented at SWW in years pasted. (

http://www.3dvision.com/3dvision-technical-support-services/solidworks-world-presentations)

4) Hire an outside source to help you get organized, trained, etc...
5) Never change the default colors in SW.

Most companies are not going to release their modeling standards, etc... because its specific to them and may not work for your needs. Its something that you or someone there needs to start creating and make sure management backs you. Because if they don't push this along, everything you do will be for nothing. If users are not told by management to follow this process, then they will continue to do what they want how they want to get work off their desk. A lot like "DiegoLGraves" points out above

quote]

Good luck sounds like your going to need it!

Scott Baugh, CSWP

http://www.SuperATV.com

GEASWUG Greater Evansville Area SWUG Leader

http://www.scottjbaugh.com

"If it's not broke, Don't fix it!"

faq731-376

 

[CorBlimeyLimey]

I don't have a checklist for you, but this website (

http://resilientmodeling.com/)

has some good information on modelling techniques.

 

[CorBlimeyLimey]

These may be more directly helpful.

http://resilientmodeling.com/BP1_Menu.html

http://resilientmodeling.com/BP5_Checklist.html

 

[duk748]

hello again & a big thank you to all who have relied & added links to help out my cause -

 

[drawoh]

duk748,

Here are some modelling rules I would like to see...

[ul]
[li]All origins, sketches and planes in the model are to be turned off when not in use.[/li]
[li]You need an understanding what what dimensions people will model to. I prefer nominal size. If you are doing rapid prototyping or some other model based definition, you may have to model at median size. Everybody should do the same thing.[/li]
[li]The best and safest way to model machined parts is to start from a block, and remove material. Don't do anything your machinist cannot do.[/li]
[li]Model all parts in the approximate colour they will be in when they are fabricated and finished. [/li]
[li]Set the material parameters, especially the density. [/li]
[li]Add the BOM information to each part right when you start modelling it.[/li]
[li]...[/li]
[/ul]

--
JHG

 

[Eltron]

How about: no mustard and ketchup allowed on the Feature Manager. This one grabs me by the pink parts every time I work on someone's model that doesn't care about errors in the feature tree.

Dan

http://www.eltronresearch.com

Dan's Blog

 

[TheTick]

Some of these "standards" are just counterproductive BS.

Machined parts cut from blocks? Maybe, if nothing you design has purpose or context...

Color? Trying to think of something that matters less...

Modeling parts to match drawing views doesn't count for much in auto and computer industries, where parts are modeled with common origins. Maybe just fire the users who are incapable of making drawing views "relative to model".

 

[jassco]

I agree with TheTick. When you design a part, you should focus on its design intents.

ASME Y14.5M specifically advises not to call out manufacturing methods on prints.

Best regards,

Alex

 

[DiegoLGraves]

Dan, tick and Alex, yup. Our latest quality initiative is asking engineering to note on the drawings all the occurrences of the shop or vendors screwing something up - like that will prevent it from happening again. Trying to keep my mouth shut here until this exciting opportunity quietly dies.

feeling passive/aggressive, Diego

 

[ShaggyPE]

I created a document a couple years ago because we were outsourcing some design/modeling/drafting to a vendor. The main purpose was to be able to point to the document when they did something that was "undesirable."

-Dustin
Professional Engineer
Pretty good with SolidWorks

 

[ShaggyPE]

Table of Contents
1.0 Purpose 1
2.0 Scope 1
3.0 Revision 1
4.0 Reference 2
5.0 Abbreviations/Definitions 2
6.0 Part Modeling 3
7.0 Assembly Modeling 4
8.0 Drawings 7
9.0 File Naming Conventions 9
10.0 System Maintenance 10
11.0 Appendix A: Drawing Samples 11

1.0 Purpose
This document defines the preferred practices for the use of SolidWorks mechanical design software.
2.0 Scope
The intent of this document is to outline modeling methods that have been found to work well in the <company name> environment as well as identify those that don’t. This document should be used in addition to good judgment based on experience with SolidWorks design software.
3.0 Revision
This is a new revision and should be read in its entirety.

4.0 Reference
4.1 WI-5-1-8 SolidWorks Workgroup Manager – User Procedures for specifics on custom property usage and general Windchill PDM interface information
4.2 \\Hydra\meteam\Standards\ OPTI_SWsettings.sldreg for importable SW settings (file locations, line weights etc).
4.3 Lombard, Matthew. SolidWorks 2007 Bible, Wiley Publishing, 2007.
4.4 ASME Y14.5 -1992, Dimensioning and Tolerancing
4.5 ASME Y14.41- 2003, Digital Product Definition Data Practices
5.0 Abbreviations/Definitions
FMT: Feature Manager Tree – The model structure of either a part or assembly file.
PDM: Product Data Management – PTC Windchill software used to manage company data.
6.0 Part Modeling
6.1 Approved Part Templates should be used.
6.2 All sketches must be fully defined.
6.3 All sketches and features must be error free.
6.4 It is preferable to use simple sketches and multiple features vs. a single complex sketch with a single feature. (i.e. a single sketch that contains the part profile, cuts, fillets, chamfers and holes is undesirable) This type of practice makes future edits of the part difficult and can actually negatively affect performance.
6.5 Feature creation should be as simple as possible. The practice of adding/removing material when a previous feature’s dimension could have been changed to achieve the same result should be avoided. (No FrankenModels). Renaming of features is not necessary, but is desirable where practical.
6.6 A minimal amount of dimensions should be used to define sketches. Sketch relations and construction geometry are the preferred method of ensuring design intent. If multiple dimensions are necessary that are intended to be the same value, the “link values” function should be used.
6.7 Make relationships to sketches rather than to faces or edges when possible (this is because faces and edges tend to lose references easily). Don’t make relations to tangent edges created by fillets (fillets are often moved, deleted or changed, which may upset your relations).
6.8 Use hole wizard to generate all holes. This is helpful in the assembly environment for patterning hardware as well as the drawing environment for hole callouts.
6.9 Use SolidWorks Weldment functionality for welded frames rather then creating an assembly with individual parts. Weldments of plates are to be modeled in a single part file as well, resulting in a multi-body part.
6.10 Material must be defined within the part file so an accurate assembly weight can be determined.
6.11 When making changes to a part (revisions) that involve editing sketches, deletion of sketch entities should be avoided. New sketch segments generate new faces and edges, thus turning dimensions brown in the drawing.  If at all possible, sketch entities should not be deleted when making this type of change.
6.12 When generating a mirror component (Left Hand and Right Hand), the Insert>Mirror Part functionality should be used… generating a new part file that is driven by the parent part file. The mirror part should not be generated in the context of an assembly. Generating a mirror part as a configuration within the primary part is undesirable.
6.13 Don’t model things that don’t need to be modeled: for example knurling, threads, and connector pins.
6.14 When the part is completed, it should not have any suppressed features, unless the suppression is for the purpose of changes between configurations.
6.15 Configurations should be controlled using a design table. Files with only minor differences between configurations and/or files with only a couple configurations may not need to be controlled by a design table.
6.16 For components that require engraved or silk-screened text, the use of extruded text is NOT desirable. See Drawings section for preferred method.
6.17 Verification and Validation will need to occur on solid models that are given or intend to be given to manufactures. This validation is not indicating that the CAD model is suitable directly for CNC manufacturing.  Additional work would be necessary to prepare the CAD model for CNC manufacturing (MMC adjustments etc). The model is simply a reference for the manufacture to use as they see fit. The drawing is still the contract document. This is not to be confused with Digital Product Description (see References and drawings section.) A note is to be added to form 4.4 (Drawing Checklist) and in PDM Meta-Data specifying that the model has been reviewed and approved for accuracy and conformance with the drawing.  Do specify revision and iteration reviewed.
7.0 Assembly Modeling
7.1 Approved Assembly Templates should be used.
7.2 The first part inserted into an assembly should be a major component. It should be fixed to the origin of the assembly. There may be exceptions to this but there should be a good reason behind the deviation.
7.3 All components must be fully constrained with the exception of hardware. Hardware does NOT require a mate to “clock” it.
7.4 A folder should be created within the assembly model called “HARDWARE”. All of the hardware should be moved into this folder. This is so the checker can quickly inspect the assembly model looking for unconstrained components. Everything outside of the HARDWARE folder must be fully constrained.
7.5 Derived Component Patterns should be utilized as much as possible. Specifically for the insertion of hardware. This is to minimize the total number of mates in the assembly. Linear and circular patterns should only be used when a derived pattern cannot. Linear and circular patterns are not driven by part geometry and therefore must be manually updated if a hole pattern changes.
7.6 The preferred method of mating parts is to follow the “real world” logic of assembly. This means mating hole patterns with concentric mates. This is a form of design check. It also helps to ensure that hole patterns get updated appropriately because mates will fail in the assembly if patterns are not consistent.
7.7 The number of top level assembly mates should be kept below 300 due to processing capabilities. If an assembly is approaching this threshold, greater utilization of sub-assemblies should be considered.
7.8 Flexible sub-assemblies should be avoided. Use of flexible subassemblies will slow things down
7.9 In-Context Design should be used sparingly. It should only be used in cases where components will NOT be re-used in other designs.
7.9.1 Keep track of your in-context use. Order your parts so references only go up the tree. Good practice is that all in-context features are based off of the first part in the assembly. The use of skeleton parts or assembly layout sketches is even better.
7.9.2 If you feel you must remove external references from parts, at least use “Lock References” instead of “Break References”. This gives you the ability to change your mind later. There is no benefit in Breaking References. If good practices are followed, there isn’t a need to lock references.
7.9.3 An in-context part should NOT be initially created within the assembly (insert > component > new part… select plane). It should first be created as a standalone part, then added and mated within the assembly. Only then should in-context features be added. This is in an effort to minimize the amount of geometry that is controlled by the assembly. It also prevents the part geometry from “being off in space” within the part file (relative to the origin of the part). This practice results in a more robust in-context assembly.
7.10 Don’t mate to in-context features, component pattern instances or assembly features. Mating to these types of features can easily cause circular references within the assembly. Causing rebuild icons that won’t go away and drastically increasing rebuild times.
7.11 Don’t mate to features that are eliminated in a configuration.
7.12 Resolve all feature and mate conflicts / errors
7.13 Distance and Angle mates should be avoided if possible unless they specifically represent design intent. Preferred methods of achieving the same result are to create planes at the part level and using a coincident mate. Distance and angle mates sometimes flip in the assembly (specifically if the assembly is large). Coincident mates to planes created at the part level are more robust.
7.14 Use Display States instead of configurations for visualization only. Display States are much faster.
7.15 For the purposes of large assembly management, SpeedPak functionality should be utilized.
7.16 Due to Windchill PDM restraints, hardware inserted must be “all there or none there” (for a given hardware part number). It is acceptable to generate an assembly model with no hardware. The hardware part numbers will be manually entered into Windchill. However if it becomes necessary to insert a piece of hardware (for stackup or detailing purposes) every instance of that specific piece of hardware must be inserted. This is because the Windchill BOM is driven by the SolidWorks model and is un-editable once SolidWorks contains an instance of a part.
7.17 Due to Windchill PDM restraints, suppression of components is unacceptable (for completed designs). Windchill doesn’t support it (no error message, just freeze). This sometimes becomes a minor issue when creating multiple configurations for the purpose of showing assembly steps or components hidden for clarity (see use of Display States). In this situation, hide should be used rather than suppress.
8.0 Drawings
8.1 Approved Drawing Templates must be used.
8.2 Drawings will conform to appropriate ANSI/ASME standards, including ASME-Y14.5-1992 (Geometric Dimensioning and Tolerancing).
8.3 Title block information is driven from custom properties within the drawing file and/or custom property information in the model file.
8.4 Notes are placed on the sheet of the drawing (with the views, but locked to the sheet), not on the sheet format.
8.5 BOMs do not exist on the drawing. Instead a label, “SEE SEPARATE PARTS LIST” is placed in the lower right corner of the drawing. The separate parts list is the product structure located within the pdm system.
8.6 PDFs should be created on the appropriate sized sheet. They should not be scaled to fit an 8.5” x 11” sheet. SaveAs pdf appears to give better results than printing to pdf.
8.7 The below list of Line Thicknesses must be used for pdf generation and hardcopy print generation:

Printer Line Thickness
Thin: .005in
Normal: .010in
Thick: .014in
Thick(2): .020in
Thick(3): .028in
Thick(4): .039in
Thick(5): .055in
Thick(6): .078in
8.8 For components that require engraved or silk-screened text, the use of extruded text is NOT desirable. The preferred method is to use sketched text within the model and then overlay annotations in the drawing file. A 1:1 scale view is placed on the drawing. Within this view, the corners of the part are identified with cross hairs. A few holes can be identified with center marks. All edges are changed to the color white. A reference dimension is also placed on the view to ensure proper scaling when printed. See Appendix A 11.1 for example.
8.9 Installation drawings or any drawing that shows a reference structure or component shall follow the below guidelines. The reference structure’s model will conform to the proper naming convention. The component line font of the reference part shall be changed in all views to thin and solid. The component shall be placed on a new layer called GRAY. The layer shall be set up such that model edges are thin, solid, and a dark shade of gray. See Appendix A 11.2 for example.
8.10 On occasion the intended manufacturing method of a component will be to use the SolidWorks model directly (ex: stereo lithography, Selective Laser Sintering etc). Reference: ASME Y14.41-2003, Digital Product Definition Data Practices. In this situation a specific details are unnecessary but a drawing must be created regardless.  It will contain an image, overall dimensions, critical dimensions, material, notes, etc.
Parts that are intended for this manufacturing method shall include a drawing with at least the following: See Appendix A 11.3 for example.
· Envelope dimensions
· Datum references
· Special feature information
· Tolerances
· Fully define/locate a select few features (e.g. holes) for the machinist to gain confidence in the program and setup.
· Material selection
· Finishes
· Special notes
· Boarder with Rev control, etc.
· A note containing the exact name of the file to be used for manufacture (including revision).


9.0 File Naming Conventions
9.1 Drawing Files: All drawing files will receive the OPTI part number only and no configuration dash number.
Drawing File Example: 1004389.SLDDRW
9.2 Single Configuration Part/Assembly Files: Part files are to be named with the OPTI part number including dash number.
Single Configuration Part File Example: 1004389-001.SLDPRT
9.3 Multi-Configuration Part/Assembly Files: Part files are to be named with the OPTI part number without a dash number. Configurations will be made using a design table where appropriate. Configuration names will be the complete part number (1004389-001, 1004389-002, etc).
Multi-Configuration Part File Example: 1004389.SLDPRT
9.4 OEM Part Files Modeled in Assemblies: This applies to OEM items such as zip-ties, hoses, and etc. that would be modeled specifically for an assembly for visual aid. These files are named first by the assembly “used-on” number followed by the OEM part number. The dash number for the assembly portion of the file name only needs be entered if it is specific to a certain configuration. A dash number can apply to the assembly configuration and/or OEM configuration.
OEM Part Files Modeled in an Assembly Example: 1005909_1002508-002.SLDPRT
9.5 Part Files such as Raw Stock: These files will be named with the assembly “used-on” number followed by a noun phrase describing what it is. This applies to anything that cannot be tied to an OEM document or drawing such as a weldment drawing that would only callout raw stock. This is the non-preferred (old) method to model a weldment therefore this filenaming is a rare occurrence. This method is more often used when a reference structure is required for an installation assembly.
Part File Examples: 1004486-001_bead1.sldprt or 1014552_GantryRef.sldprt
10.0 System Maintenance
10.1 The temp areas of your computer should be cleaned out regularly. Once a week should be ok. (C:\windows\temp, C:\documents and settings\<user name>\local settings\temp)
10.2 Know where SolidWorks puts backup and autorecover files, and clean these out when not needed (C:\documents and settings\<user name>\local settings\TempSWBackupDirectory). This location can be changed by going to tools>options>system options>backups.
When these areas become too full, Windows delays slightly when SolidWorks is trying to read or write to them, and functions can time out or crash.

Excuse the formatting from posting in the forum... but this should get you well started.

-Dustin
Professional Engineer
Pretty good with SolidWorks

 

[duk748]

hello again & a very well deserved thank you to all on this forum - the response has been very enlightening & a wealth of info has been passed along - extra kudos to shaggype for posting his great body of work for all of us - i thank you sir - i only hope that our group here will learn by this & implement what was discussed here - thank you all again & i hope everyone has a nice weekend -

 

[drawoh]

TheTick and jassco,

Machined parts have to be cheap and manufacturable, among other things. Cutting down from a block keeps you aware of what they can do easily. You are not calling out the manufacturing method, just understanding it.

--
JHG

 

[drawoh]

TheTick,

I did not mention anything about where the origins are. I had a nasty experience recently generating drawings of parts which had been modelled in place on weirdly oriented features. I had to add planes orthogonal to the parts so that I could save views that would allow me to generate fabrication drawings. Most of my stuff is machined. I do a fair bit of sheet metal, and some weldments.

In the automotive industry, with all the weird, non-ortho body features, I would expect to see different modelling techniques, especially if they are doing MBD.

--
JHG