Dezignstuff SolidWorks Blog

Yes, yes, yes, yes, maybe, definitely not, and yes…

At most of the places I’ve worked, the things that we wanted to “force” upon users, we simply set up in the part/asm/drawing templates, like planes, names, title blocks, etc. I created a standard Settings profile, and copied to all workstations. From there they could customize if they wanted to, with the exception of Files Locations, External References, Multi-User environment settings.

As far as modeling procedures, I would try to establish a document that had all that spelled out, that was accessible to everyone on the server. We would try to have weekly/monthly meetings to discuss, add to, take away from, and change that document.

A few examples of “standards” used:

*Parts to be modeled in the coordinate system as they are oriented in an assembly, ie when you go to assemble, the coordinate systems are aligned the same way. Origins, however are to be located as to make the part as symmetrical as possible w/in the part file.
*Mirrored parts are to be created using CONFIGURATIONS, using the Mirror Body and Delete Body commands, thus requiring only one part file.
*Extrusions – Entire extrusion profile goes in the sketch, including chamfers/fillets. ONE extrude features. All secondary operations go below that.
*Die-Cast/Injection-molded parts – Fillets and Draft to be applied at the END of the tree, or at least grouped as much as possible
*Detail – As much as possible, (text,threads,logos,artwork, etc)however, create another configuration, a simplified version, for use in larger assemblies. In assemblies, create a fully functional assembly, as much as possible (w/out running into issues w/ flexible mates).
*Fully-defined sketches, with more reliance on relations to define geometry, at least as much as possible. Exceptions made for surfacing operations
*Avoid some of the more taxing/fake-it features such as flex, deform, etc. The rest are more than welcome, such as split face, delete face/body, fill surface, composite curve, wrap, any of the surfacing features, etc.

As much as you want to “control” the modeling process, I think it’s really important that you give the designers freedom to do some things their own way sometimes. What’s more important is you (and everyone else) being able to use all the tools available to work with other people’s data and make it work with your own workflow and style. The more you try and fight it, the more frustrated you’ll get, because people are just plain different, and see things differently. Learn to work with it, and you’ll be better able to overcome those challenges. Sure, there are some people that shouldn’t be allowed to model, but sometimes you have to suck it up and deal with it. I spent months one time trying to “fix” this one previous employee’s crappy models. In the end I just couldn’t possibly redo ALL of his work so I just had to learn to work with it.

My $.02

I’d love to see those kinds of standards in my work place, but there are none.

What about mating standards? I work on large assemblies (2k+ parts) and without consistent mating practices, things fall apart quite quickly…

-R

Back in the days before SolidWorks, companies aspired to put into place “standards”…drawing templates, layers, plotter pens, etc…

It seems in our haste to adopt cool 3D CAD tools, we’ve fallen away from applying applicable 3D modeling standards.

Some may argue that they want the “freedom” to design and use the software how they want. I agree to a point. Ultimately, we all want Predictable Parametric Performance — Being able to edit a model (either our own or someone else’s) and not have it BLOW UP!

I guess that’s what CSWP certification is ‘supposed’ to help ensure.

Realistically, there are many modeling standards that can (and probably should be enforced)(i.e. Fully defined sketches, no external references, etc).

The real question is WHO is going to enforce them? Back in the day we had checkers who enforced ‘drafting’ standards..

My .02

BruceBuck touches on the fact users are ‘different’. Taking this into account; defining how a drawing/document(2d) should be presented is easy; to apply similar techniques to the process/function/task of creating a model whilst at the same designing a new product/machine or tooling etc. can be an exercise requiring more effort and costly control than it is worth.

A quick look at the Puffy Cube challenge is an indication of the complexity required to control modelling: and the problem is is if you say an electronic model is to be ‘modelled’ in a particular manner or using specific techniques you could well be limited the potential of both the tools being used and the ‘designer’.

I think my suggestion would be that management has to ensure their ‘modellers’ have the most complete training in the application of the tools available to ensure users can work with as wider variety of models created within a particular environment.

Back in the day with Cadkey, I had established “Standards” but when 3D came around I kind of fell away from making people follow standards. I believe that with a few lessons learned people tend to like the freedom of little standards. I would like to start looking again at some kind of “Standards” because I’m thinking more and more people will want to follow ASME Y14.41 – 2003 in the near future.

My $.01 (I’m going to have to give my other $.01 to our Government)

As far as the question regarding WHO should enforce, it’s easy to say, the CAD Admin, or management. However, what it REALLY takes, is finding someone WHO CARES. And therein lies the problem. Too many people don’t care. They’re just there because it’s a job; they’re not really driven or motivated by what they do.

I takes someone who cares about the group working together and being more efficient to head up the effort to create a standard and attempt to enforce it. Sad, but true.

As far as mating standards, yes that’s also part of it. Ours were as follows:
*ANY cylindrical part is to have an AXIS feature at the top of the tree. This Axis feature is to be used for mating. This includes Toolbox parts.
*Try to mate components using its primary datums, when possible, and when it makes sense. Sometimes it makes more sense to mate to a face or and edge (in order to make it function, or preserve design intent), but MOST of the time, it just creates problems when the part gets changed or revised. PLUS, it will aid GREATLY when swapping out that component for a different one using Replace Components.
*RENAME mates in larger assemblies, especially when they involved mates for RH/LH types of configurations. If the mate is only used in the RH assembly, tag the letters “RH” on the end so it will be easier to find,suppress, etc.
*Limit mates are cool, but seems to be buggy as !@#$ (at least 2007 and earlier), especially when trying to use flexible assemblies. Go ahead and creat different configs (usually derived configs, leave the parent as the “flexible” version )for the different assembly positions (Open/Closed, Extended/Retracted, etc.)

Oh, and regarding the AXIS feature, it is NOT created by selecting a face. It’s created using the intersection of those primary planes (Front/Top/Right). This will ensure that no matter what happens so the geometry, the mate won’t break. This would require people to model the component based on its primary pivoting point.

I developed a standard ref. guide, but it’s not being used by every user. In there is stuff like naming features, fillets at the end of the feature tree. Stuff like that. I guess it’s mostly a best practice guide but it’s there for anyone to use.

The information listed below is the “short version” of a document used to train SolidWorks users on specific requirements and procedures. The “long version” contains contains hyperlinks to another ten associated documents. I apologize for some of the formating that did not copy properley. If you are interested in the original document, e-mail me at “edward.cyganik@itt.comREMOVE”

“SolidWorks Reference Guide”
This document should be utilized during creation and as a final review of all SolidWorks objects, Parts, Assemblies & Drawings. For ease of use, the Check List below contains links to expanded or example information found throughout this document and to related external documents. For additional information, refer to the SolidWorks User Guide, On-Line-Help and the Engineering Data Index that contains links to wide variety of related documents.

Check List

1. GENERAL: Go to “GENERAL” Section
1.1. Are your SW options and external references correct and up to date?
1.2. Are you using and maintaining proper directory structures?
1.3. Is local company data backed up on a network drive?
1.4. Are you working locally in your own directories?
1.5. Do you know your working environment? Are you comfortable with all interfaces?
1.6. Is the computer doing all the work? Are you an active participant?
1.7. Are you maintaining your computer properly?

2.ALL OBJECTS: (Parts, Assemblies & Drawings) Go to “ALL OBJECTS” Section
2.1. Is the proper template being used for …
2.1.1.… Parts?
2.1.2.… Springs?
2.1.3.… Assemblies?
2.1.4.… Drawings?
2.2. Is the naming convention correct?
2.3. Have proper values been filled in for all Custom File Properties? If they don’t exist have they been created?
2.3.1.… Parts & Assemblies?
2.3.2.… Drawings?
2.3.3.… Springs Drawings?
2.4. If equations have been used; Are there any errors? Are they correct? Do they make sense?
2.5. Check the FeatureManager Tree (FMT) to verify that the object has been rebuilt.
2.6. Are all items the proper color? Everything is not Black & White.
2.7. Orient to a descriptive view, for all SolidWorks Objects.
3. SKETCHS: Go to “SKETCHES” Section
3.1. Have the default planes been used where ever possible?
3.2. Are Dimension & Geometric Relations attached to the correct entities?
3.3. Have you minimized requirements for sketching and reduced the probability of errors?
3.4. Has design intent been captured?
3.5. Are sketches geometrically correct and properly dimensioned?
3.6. Is the sketch proper for feature to be created?
3.7. Have construction aids been used to define sketches?
3.8. Have base features been utilized for sketches?

4. ALL MODELS: (Parts & Assemblies) Go to “ALL MODELS” Section
4.1. Is more than one component fixed?
4.2. Does the FMT contain minus signs, plus signs and/or question marks?
4.3. If configurations exist, were they created properly? Are they correct? Have Design Tables been incorporated?
4.4. Are exploded views and/or 3D views available?
4.5. Has the model been reviewed?
4.6. Has the model been visually inspected?
4.7. Have external references been reviewed?
4.8. Would a temporary drawing aid in the design process?

5. PART MODELS & FEATURES: Back to top of Check List or Go to “PART MODELS & FEATURES” Section
5.1. Has the part been created to suit the manufacturing process? Also see: ENI_DFM.doc
5.2. Has the part been created to suit assembly needs? See: ENI_DFA.doc
5.3. Have features been aptly named? ()
5.4. Is an “Alter Item” or “As Manufactured” part model required? See AlteredItems_BaseParts.doc & AM&A_MODELS.DOC
5.5. Has the part been constructed smartly?
5.6. Has the Hole Wizard been utilized where possible?
5.7. Have Library & Palette Features been employed?
5.8. Have the following items been created or setup in the part mode …
5.8.1. … Material Density?
5.8.2. … Reference Dimensions?
5.8.3. … Tolerancing?
5.8.4. … Annotations? (Notes)
5.8.5. … Cosmetic Thread Callouts?
5.8.6. … Surface Finishes?
5.9. Are there suppressed or hidden features in the FMT?
5.10. Is the display correct for all sketches, planes, axis, points, etc.?
5.11. Have requirements for Part Configuration been considered?
5.12. Do you have a robust Part Model?
5.13. Have Text Features been minimized?

6. ASSEMBLY MODELS: Go to “ASSEMBLY MODELS” Section
6.1. Is the assembly modeled properly?
6.1.1. … Proper Base or First Component?
6.1.2. … Use of Neutral/Symmetry Plane?
6.1.3. … Proper use of Sub-Assemblies?
6.1.4. … Required Assembly Features?
6.1.4.1. Is an “Alter Item” or “As Manufactured” assembly model required?
6.2. If required at drawing level, have the following items, been created in assembly mode for later use…
6.2.1. … Isometric or 3D Views?
6.2.2. … Exploded Views?
6.2.3. … Weld Symbols?
6.2.4. … Surface Finishes?
6.2.5. … Reference Dimensions?
6.2.6. … Tolerancing?
6.3. Are there suppressed, hidden or lightweight, “out-of-date” components in the FMT?
6.4. Are there any suppressed mating conditions?
6.5. Do the terms or appear as suffixes on any components in the FMT?
6.6. Have all requirements for Assembly Configurations been satisfied?

7. DRAWINGS: Go to “DRAWINGS” Section
7.1. Has the drawing been setup properly?
7.2. Has the display been set for all items in all views?
7.3. Are all proper/required model dimensions displayed?
7.4. Have driven (reference) dimensions been kept to a minimum?
7.5. Have true model dimensions been captured in hole call-outs and general & FOD notes?
7.6. Has the annotation “Hole-Callout” been utilized where possible?
7.7. Have all drawing items been created in the proper view, sheet or template?
7.8. Have the general notes been created properly?
7.9. Have the proper Blocks been used?
7.10. Have View Inserts been utilized?
7.11. Is the Design Table correct? See DT_SW&ST_Contents&Appx.ppt
7.12. Is the Bill of Material correct?
IF IN DOUBT ABOUT ANY OF THESE PROCEDURES, ASK FOR ASSISTANCE!

 GENERAL: Back to Check List
 Support Files;
 Properly maintain your Option File. SWOP2006.reg & sw_options_2006.doc
 Organize & manage your data & external references.
 Proper Directory Structure;
 Create appropriately named directories.
 Do not place any files or create any directories (working or personal) in any application directory.
 Segregate files with adequate sub directory structure.
 Backup all current or in process data to the proper network drive.
 Work in YOUR directories ONLY. DO NOT work in any of your neighbors’ directories.
 Perform maintenance regularly. (Review/Remove temp files, delete back up files, etc.)
 Get to know the environment & the GUI’s for WINNT, SolidWorks, SmarTeam, etc.
 Be aware of what is required; a menu pick, an input to a pop up menu, a screen pick, etc., use Help menus.
 Message windows are exactly what their names imply, delivery of messages, some good & some bad. In any case, you should pay attention to this portion of the GUI:
 A feature is created but does not display or you do not see it;
 Was it created at all? Was it aborted? Was it created with an error?
 Was a failed feature inadvertently suppressed during a rebuild or in the feature creation process?
 A component is assembled but does not display or you do not see it;
 Was it assembled at all? Was it aborted? Was it assembled with an error?
 Was a failed component inadvertently suppressed during the rebuild of the assembly or during the insertion of a component in the assembly process?
In ALL of the cases mentioned above, the message window would have displayed a response or status. Always be aware & review accordingly.
 Actively watch or review the regeneration process of parts, assemblies & drawings. This can be done…
 … during initial retrieval. (all objects are regenerated)
 … after a modification is made. (from point of modification to the end)
 … when you roll back the feature manager. (from the top of the FMT to the Rollback location.)
 Review the feature manager tree, then justify or resolve the following;
 Are all minus signs (-) acceptable?
 Over defined items, indicated with a Plus sign (+), must be resolved.
 Items that cannot be solved, shown with a Question mark (?), must be solved.
 First component in an assembly can be fixed (f) all other fixed components must be scrutinized.
 Resolve all Red Exclamation Marks (!), follow the Red Arrows ().
 Review All External References () and Resolve if necessary;
  Normal External Reference
 ? Out of Context, External Reference not Up-To-Date. (Load Model)
 * Locked External Reference (Not a normal practice. Why is it locked?)
 x Broken External Reference (Unacceptable.)
 Review your computers and personal working directories prior to start & at the end of a session.
 Delete all unnecessary files. Keep your directories clean, including:
 Using the SmarTeam Local Files Explorer, keep “C:\Work” clean.
 After a crash delete all SW temp files, files = “~$FileName.sdlxxx”.
 Periodically cleanup files in the temporary SW backup directory, files = “Backup of FileName.sdlxxx”.
 Clean up the “Temp” directory, “C:\Documents and Settings\login-name\Local Settings\Temp”. Delete all “*.tmp” files and all temporary files generated by using SolidWorks, SmarTeam, the SW Viewer from SmarTeam.
 Clean up the “Temporary Internet Files” directory.
 For detail on all of the above, see: Maintenance&Performance.doc

 ALL OBJECTS (Parts, Assemblies & Drawings) Back to Check List
 Start objects as follows: SeedObjects.doc
 Create parts using: Enidine Start Part.prtdot (or “ISO_” part templates)
 Create coil spring parts using: Right-HandCoilSpring or Left-HandCoilSpring.prtdot
 Create assemblies using Enidine Start Assembly.asmdot (or “ISO_” assembly templates)
 Create drawings using ASIZE, BSIZE, CSIZE, DSIZE, CoilSprg, CoilSprgS, CoilSprgCG, or CoilSprgSCG. (or ““ISO_” or “CMC_Enivate_”.drawing templates)
 Create all parts, assemblies & drawings using the proper naming convention by referring to the Enidine DRM, ES-3000, the Part Number Code Book (PNCB) and to any approved group or department specific documents.
 Fill in values for Custom File Properties as follows:
 For Parts & Assemblies: cust_part+assy_props.doc & ModelProps.txt SW_CoilSpring.doc
 For Drawings: cust_drawing_props.doc
 For Coil Spring Drawings: CoilSprgDrwInst.doc.
 Use TOOLS/EQUATIONS/EDIT ALL to verify that there are no errors. Have dimension names in equations been given understandable & meaningful names? If not, consider adding equations to ensure proper rebuild and minimize the number of manual edits required. “Equations – Useful Math Functions & Operators”
 If there is any RED in the FMT of any object, errors must be resolved. Rebuild (CTRL B) or forced rebuild (CTRL Q) to fix all problem areas. No RED (Bleeding) exclamation marks (!) or arrows () are acceptable.
 Everything is not black or white, colors have the following meanings: SW_Color_Codes.doc
Check the color of Dimensions, Notes, Sketch Entities, etc. to verify proper status, only Black is acceptable.
 Black. = Satisfied
 Blue = Under Defined
 Red = Over Defined
 Brown = Dangling
 Pink = Not solved
 Yellow = Invalid
 Driven = Gray
 Prior to saving databases, orient to a descriptive view, shade and then zoom to fit. For drawings, zoom to fit is all that is required. This technique provides for proper viewing when using the File Open dialogue box, Quick View and the SmarTeam viewer.

 SKETCHES:
 If possible, use the existing planes (Front, Top & Right) for sketching & orientation. Dimension to these planes and the origin whenever possible.
 Dimension & Add Geometric Relations to what is required and not what happens to be picked or assumed to be picked. Perform these tasks;
 while in an isometric view, rotate to an advantageous view and/or use HLG display.
 using select other.
 by selecting from the FMT.
 To avoid unnecessary sketching and reduce the possibility of errors, use Predefined, Copied or Derived sketches.
 To capture design intent, use edges, offset edges, dimension to edges and apply geometric relations to edges where possible.
 Modify sketch by Dragging an Entity or Vertex to verify or determine proper movement/design intent then Add/Change the Dimension Value for verification.
 Use “Tools/Sketch Tools/Check Sketch for Feature” to verify proper sketch to feature type.
 Use centerlines, construction arcs, points, etc., to aid in solving/defining sketches.
 Relate as many new sketches as possible to the models’ base features. Using this method will reduce the number of parents involved and therefore reduce modification and rebuild errors.

 ALL MODELS: (Parts & Assemblies)
 The FMT shall contain only one fixed (f) component. If more than one component is fixed, there must be justification.
 Check the FMT. Are Minus signs (-) acceptable? Plus signs (+), denotes over defined. Question marks (?), mean something could not be solved. Investigate all cases and resolve as necessary.
 If a model contains configurations, check for proper names of all configurations. All families of parts and assemblies must be Design Table driven. Items in the internal MS EXCEL table should be given meaningful/understandable names, these item include, dimension symbols, feature names, parameters, etc.
 Provided for exploded and/or 3D views by creating, naming & saving properly.
 Review the creation process by using the Rollback Bar. Look at the modeling techniques that were utilized, possible errors & sound practices.
 Visual interrogation of a model can reveal a wide variety of problems. Shade the model & view from numerous directions. Many times a misplaced item (feature or component) will show up as a flaw in a shaded image. Conflicting volumes can also be detected in HLG/HLR views. Reviewing the surface topology of any model can sometimes result in finding errors that have gone undetected.
 Any model that contains external references or is an external reference for another part must be reviewed by critiquing relationships, dependencies & references. The Parent/Child pop-up menu and the File Find References command can be used for investigation. If any of the following items are found in the FMT , ?, * or x, then RMB on the item and select List External Refs, then investigate as necessary.
 In order to perform measurements and/or to better visualize a design, it may be beneficial to create a temporary drawing. If a temporary drawing is created, it can easily be modified to satisfy requirements for production drawings.

 PARTS MODELS & FEATURES:
 Map out part modeling strategy prior to start. Do this by determining…
 … what manufacturing process will be (lathe, mill, cast, forged, molded, sheet metal, etc.). If a part is created on a lathe, start with the proper bar stock. An extrusion should start out with the proper extruded shape & size. The Overall Finished Dimensions are all that is necessary to simulate stock size. Extra material shall not be added.
 … the base (first) feature type (extrude, revolve, swept, blend, advanced, solid, thin, etc.). It should provide for the most bang for the buck, it should be the most stable.
 … if a neutral plane or axis feature would be helpful.
 If this is the case, refer to the Part Number Code Book, the Enidine DRM, ES-3000 and associated materials pertaining to “Altered Items” or “As Manufactured” models.
 As a minimum, key features should be given meaningful names for quick and easy identification.
 When necessary, take advantage of creating construction features such as planes, axes & points and/or use sketch entities to aid in a design process. Any construction aids should lend themselves to capturing design intent. As new features are created & added, dimension & align them to surfaces, axis, planes & edges which make sense. Perform these tasks while in an isometric view and/or by using select other.
 If possible, create all holes using the Hole Wizard for addtional benefits at the drawing level (Hole Callouts).
 Library & Palette Features should be used whenever possible. To decrease modeling time, consistently dimension common features and reduce the possibility of errors, see LibFeat.doc & LibraryFeatures.xls
 Determine & then create or setup the following part model items;
 Material Density (For precise weight calculations.) See the “Density Tab” in ENI_STD_NOTES.xls
 Reference Dimensions should be created in the part model where required but should be kept to a minimum. Excessive use of reference dimensions is a sign of poor modeling practices. Consider changing the dimensioning scheme of sketches to reduce the number of reference dimensions.
 Add all tolerances in the part model. This is where the definition of form, fit, design intent, manufacturing requirements are determined. Setup all tolerance types, nominal, plus/minus, limits, symmetric, GD&T, datums, basic dimensions, etc., in the part model.
 Annotations or Notes can be created at the part level also. If holes are created using a variety of features (versus the Hole wizard) then use the Annotations command to capture the required information so that parametric notes can be used downstream in drawings.
 During the process of creating Cosmetic Threads, be sure to fill in the Thread callout box to provide for the required notes on drawings.
 Like all other annotations, Surface Finishes should be added at the part level.
 All suppressed (gray) or hidden (wireframe) features in the FMT must be investigated and resolved. Suppressed and/or hidden features are only acceptable if there are configurations present and the state of the features are controlled in a design table.
 Investigate and set the proper display for all sketches, planes, axis, points, etc. This is a simple matter of determining whether an item is to be Shown or Hidden.
 Part Configurations should consider the following;
 Create Design Table with column headings for ease of use.
SW Help Pages: Summary of Design Table Parameters, User Notes & Comments.
 Properly name the default part and file or database name.
 Make sure your default/generic part model is robust, correct & flexible.
 Identify items to be added to the design table. Modify dimension names suitably, aptly name features, etc.
 Verify all configurations upon creation.
 A robust part can handle drastic changes. To determine if your models have what it takes, “Flex the Part”, do this by realistically modifying a random number of values on the part. If failures occur, determine the cause & correct.
 Keep Text Features to a minimum, embossed or engraved text carries a lot of overhead. SW_Txt_Feat.doc Consider creating text at the drawing level by associating any text/identification requirements to drawing views.

 ASSEMBLY MODELS:
 Map out assembly modeling strategy prior to start, by determining …
 … the base component. If a damper is to be created, do not start with a bearing, start with the shock tube or cylinder. The first component should be the most stable/dependable component in the assembly.
 … if a neutral plane or axis feature would be helpful. For assembly purposes, assembly planes and/or axis have an advantage over part features in that the Parent/Child relationship is less likely to become an issue.
 … if sub assemblies need to be created. Caution: Sub-Assemblies are not to be created for the sake of SolidWorks. Sub-Assemblies, separable or inseparable, are created to provide for logical manufacturing processes, assembly processes and spares or for the procurement of items.
 … requirements for subsequent configurations.
 … If assembly features are required, will they be created at …
 … assembly level? There are limitations that may prevent the use of Assembly Features, namely, assembly features are restricted to removal of material. To add or deform material, refer to the Part Number Code Book, the Enidine DRM, ES-3000 and associated materials pertaining to “As Manufactured” models and “Altered Items”.
 … part level? For simulation of Assembly Features that are created at the part level, again, refer to the Part Number Code Book, the Enidine DRM, ES-3000 and associated materials pertaining to “As Manufactured” models and “Altered Items”.
 … both levels, Assembly Features combined with features created at part level? Ask for assistance.
 Determine & then create or setup the following;
 Isometric or 3D Views should be created, named and saved.
 Exploded Views should be created, named and saved. This would require the creation of a assembly configuration that would also need to be named & saved.
 Weld Symbols requirements should be handled during the design stage. Identification of weld joints and types of welds should be done in the assembly model.
 If machining takes place at the assembly level and a machined area requires a Surface Finish, then the annotation should be added at the assembly level.
 If required, Reference Dimensions should be created in the assembly model and similar to part mode, they should be kept to a minimum. Excessive use of reference dimensions in an assembly may have an undesirable effect.
 For the most part, tolerances added in an assembly model would only apply to the dimensions of assembly features. When required, setup all tolerance types, nominal, plus/minus, limits, symmetric, GD&T, datums, basic dimensions, etc., in the assembly model if they will be required at the assembly drawing level.
 All suppressed (gray), hidden (wireframe) and/or out-of-date/lightweight (feathers w/stripes) components in the FMT must be investigated and resolved. Suppressed and/or hidden components are only acceptable if there are configurations present and the states of these components are controlled in a design table. Out-of-date components must be brought up to date by opening and resolving.
 All suppressed mating conditions must be investigated and resolved. Expand MateGroup Icons in the FMT and look for Grayed-out Paperclips, these denote suppressed mates. Suppressed mates are only acceptable if there are configurations present and the mate suppressions are controlled in a design table.
 It is unacceptable to have any components with the suffix or . If either one of these appear in the FMT, they must be resolved by setting the components configuration to a properly defined configuration name. Management of any configurations shall be done using a Design Table.

 ASSEMBLY MODELS: (continued) Back to Check List
 Assembly Configurations should consider the following;
 Create Design Table with column headings for ease of use.
SW Help Pages: Summary of Design Table Parameters, User Notes & Comments.
 Properly name the default assembly and file or database name.
 Make sure your default/generic assembly model is robust, correct & flexible.
 Identify items to be added to the design table. Modify dimension names suitably, aptly name features and verify that all component names are valid. Additionally, identify mates and mates with dimensions (angular and/or offset) and properly rename them for easy identification and use.
 Verify all configurations upon creation.

 DRAWINGS:
 Map out drawing strategy prior to start, by determining…
 … what views are necessary. Are they available in the model?
 … what scale is to be used. The “overall scale” is determined by the drawing’s “sheet scale”. A “View’s” scale is defined in the “Drawing View Property” and is used as an exception to the overall drawing scale only! The drawing’s “sheet scale” is the predominant scale.
 … the size of the sheet or format required.
 … if multiple sheets are required.
 … is a Design Table to be input on the drawing?
 … is a BOM to be input on the drawing?
 To best depict models, determine the proper display mode to be used for all views. In addition to view display, component & edge display mode must also be considered and set for all views.
 Verify that all required dimensions are displayed. The vast majority of a drawing’s dimensions are to be “Model Dimensions”. To verify dimensional requirements, use Insert-Model Items and select all annotation types. Use the Undo command as necessary to display properly once dimensions have been checked. (Good idea to save the drawing prior to checking.) NOTE: The proper technique for annotating a drawing is to insert model items and “hide” those that are not required. By using this technique, verifying required dimensions is easily accomplished using the Hide/Show Annotations command.
 Add reference (driven) dimensions only when necessary. If excessive dimensioning is taking place at the drawing level, there is likelihood that a dimensional scheme should be changed at the model level.
 If holes are created using a variety of features, then use the Annotations/Note command and select model dimensions to parametrically capture the information. This process must also be used to properly capture information for General & FOD notes.
 If holes are created in a model using the Hole Wizard or Insert/Feature/Hole/Simple, then use the Annotations/Hole Callout command to generate the proper notes.
 Associate items to the proper View, Sheet or Template. Do this by activating the required view or by specifically editing the drawing sheet or template as follows:
 Views (captions, unattached dimensions, notes, lettering, labels, cosmetics, etc.)
 Sheet (tables, BOM, etc.)
 Template (general notes, title block and revision block information)
 Note: To save all drawing changes, save the drawing file only. Never save the template!
 Check for the proper display of Cosmetic Threads, Datums, Datum Targets, Feature Dimensions, Reference Dimensions, Geometric Tolerances, Notes, Surface Finish & Welds. Do this by using the Annotations Folder Options or the Menu Options under Insert/Model Items.
 Use the proper/approved company notes for all company documentation and keep notes as one item, not separate entries for each note. ENI_STD_NOTES.xls Also, utilize the Unicode Character Map for non standard characters, see ExtendedCharacters.doc
 Use the proper/approved company blocks for all company documentation. SW_Blocks.doc
 Use the proper/approved company view inserts for all company documentation. ViewInserts.slddrw
 Design Tables should be sized and placed correctly. Be sure that the MS Excel file has been sized to display all required information, WYSIWYG. If design tables become large and unruly, see ManagingLargeDesignTables.doc
 Use the proper SolidWorks “Table” based Bill for BOMs. (Replace MS EXCEL BOMs when possible.)
 For most BOMs, use “EnidineBOM.sldbomtbt “ (MS EXCEL not for new design.)
 For BOMs containing “bulk items”, use EnidineBulkItemsBOM.sldbomtbt (MS EXCEL not for new design.) Also, refer to BOM_Settings.xls for instructions.
This is just an example, click HERE to go back to the Check List.

@E.L.Cyganik
Dear Sir,
I’m very pleased to see that I’m not the only one who thinks like you.

I’m very interested in the full document.
Ams would like to ue it in a Dutch translation

Thanks in advance Fred Bruintjes