SWW09: Focus Groups (Drawings and Sheet Metal)

As previously mentioned, I attended two focus groups (also called roundtable discussions) this year.  These are generally held on Sunday before all the major SolidWorks World activities begin on Monday.

Sheet Metal

The first group I attended was for sheet metal functionality.  Though attendence was very light, the number of different methodologies and opinions was high.  My own interest in the topic is the problem with being forced to use assemblies to fully document sheet metail parts with inserts.  This is an issue because if you start a drawing of a part, you cannot later replace that part with an assembly.  So, if you create a sheet metal part with no inserts and then you need to add inserts on some later revision, you are forced to recreate the drawing practically from scratch.  This is a horid time and resource sink.

Others in the group talked about using K-factors to determine the material used by the sheet metal part (for flat patterning), while others disregarded K-factors in favor of bend reduction techniques.

One request that seemed to get common acceptance is the idea of creating a table of all the bends of a part with their full characteristics, with the ability to highlight each bend by clicking on it within the table.  When this table is on a drawing, it was suggested that details be added to a specific layer.

The session  also revealed that some used work arounds to use the SolidWorks model to instruct sheet metal tooling to perform certain actions (either via direct or translated input).  Some use alternative features which do not match the final design in order to instruct a tool to produce the feature desired in the final design.

One work around solution did come out of this session.  Right now, the material mass number changes from bent state to flattened state.  Although this difference is minor, over a large quality of parts, the error multiples and can create issues in part handling.  Use a non-configuration custom property to link to the the material property (of a specific configuration?).  Use this custom property as the source for the mass regardless of the configuration or part state.


A large portion of the drawings discussion revolved around printing and saving issues with Drawings.  It seems many people are experiencing similar problems.  When saving as a PDF, views randomly disappear.  When printing as a PDF, text locations get shifted.  Also, changes to parts at lower levels of an assembly may cause errors and view changes in higher level assembly drawings; meaning the the company has to open up all levels of a product’s assemblies to make sure that any change did not affect the drawings in unexpected ways.  It seems more people are having these kind of issues that I originally thought.  Many of the problems are magnified by use of PDM’s.

The meeting also focused on DimXpert and how to handle its dimensions.  One comment is that it should place dimensions per current standards within the model.  Another comment noted that datums and feature frames should drive the model.

I voiced my other major concern as well.  Symbols from the Gtol.sym library file should be stored within a drawing.  Right now, I cannot give native drawings to others outside of my organization because they will not be able to see symbols that we employ.  When a symbol is used within a drawing, it should be included in that drawing’s file and not require editing of any other user’s Gtol.sym file.

SWW09: Skeletons and Modelling Horizontally (live, nearly)

I’m rudely blogging live from a breakout session.  Of all people, it’s Matt Lombard I’m doing this to.  He will appreciate the ironic nature of this activity.  Will he hate me for it when he finds out?  No, unless my typing annoys him right now.

OK, I’m far enough back in the room where this doesn’t seem to be an issue, though there may be people around me that might be annoyed.  Again, no one seems to care.  (If the person next to me is trying to hint to me to stop by clearing your throat, let me apologize now.  Anyways, here we go!)

Matt says people are error phobic.  They worry if they have errors in a model.  This may cause unnecessary worry about finding errors in models.

Horizontal modelling is taking things to the extreme to protect your modelling data to avoid errors in the model.  Someone interested in this type of modelling approach is interested in trying to solve a problem they are experiencing.  The two methods to address such problems are to 1) ignore them when they crop up, or 2) presumptively stop daisy chaining references.  Link to objects that don’t break, such as sketches and planes.  Don’t link to solid faces, edges and vertices.

He compares a model created through regular practice with the same part modelled with horizontal modeling.  The relationships between features are all over the place with the regular methods, compared with clean results from horizontal modeling.  In the HM model, origin planes form the foundation, when are linked to reference places, then linked to reference sketch, with independent features that are all linked back to the reference sketch; at the end are the fillets.

Design intent is described by the edges.  HM allows one to lay out design intent with a set of sketches.  Features created from this will not fail if they are re-ordered (except for fillets).  Matt then demonstrate that HM doesn’t work quite by accident, so we continue the demonstration “theoretically”.  I think the failure to achieve the desired results shows just how hard it is to implement HM effectively.  Thank god watching Matt is entertaining because this type of issue in any other session would result in very boring dead time.  Matt actively engages the audience, which is now trying to address why SolidWorks created unintended relationships in his demonstration model.  Going through this process is interesting, but distracting.

In a question from Matt about who is using HM, the audience answers.  One person states they use HM for multiple configuration components, but would not bother in a simple single configuration part.  Another individual states it is also useful in in-context model assemblies.  HM may also be useful in 2D drawings.  Of course, now the audience is trying to discuss the demonstration model.  There doesn’t really seem to be a consensus; again pointing back to issues with trying to employ HM.  Of course, maybe that just means there are more than one way to achieve stable HM.

HM models are modelled to live forever through changes.  Concept modelling may not be able to employ HM techniques since the part may not be fully understood at the time when modelling is started.

In an almost conclusionary lament, Matt states that everything in SolidWorks is like a balance between stability versus speed of use.  Using HM modelling techniques is a tool to use at the appropriate situation, such as well understood production items where the design is complete before modelling begins.

OK, just for the record (Matt), the only reason I’m live blogging is because I really do not have the time to get all the articles done that I want to this day.  I promise I will not do this in the future.  Thank you for your presentation.

Virtual Sharps

In the past, I’ve settled on using the phrase “TO V.S.” after a dimension which is to a virtual sharp.  I’ve seen this type of referencing used elsewhere.  Another set of initials I’ve seen used is TSC, which I guess stands for theoretical sharp corner.  I think this is likely older wording.  I used to like the shorter “VS” myself because it refers to what I would consider a more common term.  However, none of this matters too much since the standards say nothing about what is proper.  ASME Y14.5-2009 uses the term Point Location, but doesn’t specify any identification symbols or abbreviations for this concept.

SolidWorks graciously offers a multitude of marks to create an identification of a virtual sharp.  The main problem I run into with SolidWorks and this function is that I’m working in drawing scales or with radii sizes that frequently make such marker nearly invisible without a magnification glasses.  The other problem is that none of the marks are identified in any standards.  Heck, a third problem is that fact that the functionality is extremely hidden.  You have to know how to make a virtual sharp mark because there’s not button, or icon specifically for it.  It’s a short series of steps that would be nearly impossible to guess at.

Those steps being (within a drawing): 1) Select each of the two object lines that intersect in space. 2) Select the Point function.  How is anyone to know intuitively to select the Point function? Hmm.  Anyway, at least SolidWorks offers some method.  That’s more than can be said about the standards.

I guess I should ask what are others doing to identify dimensions that are to virtual sharps?

Here is an  updated article about Virtual Sharps.

Challenges in Transitioning from 2D to 3D

The CAD industry is so far along now that the discussion for many is no longer 2D CAD vs 3D CAD, but methodologies within the 3D CAD (such as direct modelling vs history modelling).  However, the adaption of 3D CAD applications such as SolidWorks is still on-going.  Many companies are still using 2D CAD applications.  Why does it take so long for many companies to make the transition when the benefits of 3D CAD seem to be so apparent?

I think Jeff Ray, CEO of DS SolidWorks Corp, properly identified this problem in an interview for the recent article CAD Tools: Breaking Barriers by Linda L. Bell (NASA Tech Briefs, Jan 2009 issue).  In part, he states that when a company considers making the transition to 3D CAD “the pain of change has to be less than the pain of the status quo.”  3D CAD still needs to be easy to access and use.  It also needs to be robust enough to be a design tool for those users that demand more from their applications.  On speaking about how SolidWorks has answered the need to make this transition easier, Ray states, “our last two releases have included a new user interface [where] the workflow predicts which tools the users will need and makes them readily available.”

Even still, there are many challenges to making the transition.  These involve learning a whole new way of working.  For example, when one draws a square, it doesn’t stay a square.  It can become a cube, rectagular rod or a plate.  It can also become a recess or square hole in another feature. 

Once one gets a grasp on these concepts, setting up the new 3D CAD software to work within the company’s documentation system can seem even more challenging.  This is one area that seems to missed (or at least not implemented fully) by many of the 3D CAD applications.  Having the ability to make drawings isn’t the end of it.  Communication with PLM’s and ERP’s is just as important in many companies. 

As my friend Chris MacCormack has recently pointed out, management of the 3D CAD files themselves must also be addressed.  With one or two users, this matter solves itself with simple use of folders.  However, as departments expand and companies grow, solutions for the raising difficulties change.  Of course, this must also be addressed with 2D CAD applications, but it is a much more complex matter with 3D CAD applications.

Most of us first address these issues with wide-eyed innocence. Upon going through this once, that becomes innocence lost.  To consider the transition from 2D CAD to 3D CAD, all of the above must be taken into consideration, and actually other issues too.  To improperly paraphrase Uncle Ben, with the great power enjoyed with the use of 3D CAD comes great responsibility in how it is used.

Now, it is understood that 3D CAD applications are not useful to all CAD users.  But if the field is mechanical engineering, it is very likely 3D CAD going to be worth the transition from 2D.

Assembly mates and rebuild times

A recent discussion I had with Chris MacCormack was about how mates within an assembly affect rebuilt times.  He posed a question to me.  Do I fully contrain screws after I insert them?  My answer was basically “yes, as time allows.”  He then stated that he actually promotes the notion of not fully contraining screws.  He went so far as to suggest it would be better to suppress the mates altogether and fixing all components. 

His reason for this policy is that a higher number of mates will slow down rebuild times because SolidWorks has to caculate each mate on every rebuild.  My primary thought is that I prefer my model assemblies to be stable and predictable, which full mate constraint methodology delivers.  Secondarily, on instinct, I was working under the idea that having everything fully constrained helps SolidWorks work out all the details so it doesn’t have to spend so much time figuring everything during a rebuild.  (I was aware that particular kinds of mates do slow down rebuild times.) 

So, I decided to put this to a test.  I created the model assembly shown here.  Though these are not real world parts, they are created and assemblied using real world techniques, with details I would normally use, even to the degree of adding material to each component.

Test subject

I created a series of configurations of this assembly in various states of mating, both with patterned components and with all instances of hardware individually inserted.  I then used handleman’s latest macro, Rebuildtimes.swp (which he recently provided on eng-tipsc.om as a response to a request by another user).  This macro was used several times on each configuration.  Here are the best times for each.

Condition:  First rebuild time (s)
Patterned Fully Constrained:  0.3438
Patterned Partially Constrained:  0.3125
Patterned Not Constrained:  0.2812
Patterned Fixed:  0.2656
All Instances Inserted Fully Constrained:  1.125
All Instances Inserted Partially Constrained:  0.5938
All Instances Inserted Not Constrained:  0.2656
All Instances Inserted Fixed:  0.2656

The test results show a clear pattern.  Chris’ assessment is correct.  With each additional mate, SolidWorks takes more time to rebuilt the assembly.  Even in this small example, there is a significant difference between fully constrained hardware and hardware that was just inserted via smart mates (partially constrained); 1.12 seconds verses .59.  The rebuild time was literally doubled just by adding parallel mates to fully constrain the smart mated hardware.

Even in light of this realization, I do not advocate suppressing all mates and fixing components.  In my experience, this isn’t practical for the real world.  However, this is going to make me reconsider just how I will be handling mating schemes.  There needs to be a balance between the speed of the software and the functionality of the model assembly.  Where is that balancing point?

Drawing Revisions and PDMWorks (Part 2: Automatic Revisions)

With PDMWorks, it is possible to automatically revise a drawing’s title block and revision block upon check in.  Three things are necessary to use this functionality.  First, the drawing template will need to employ a SolidWorks Revision Table.  If someone is not familiar with how to set up revision tables, please see my previous article: Settings Up and Using SolidWorks Revision Tables faster. Second, the drawing template’s title block will need an annotation note that is linked to the custom property “Revision”.  If someone is not familiar with how to link annotation notes to custom properties, please see my previous articles about this subject:Introduction to SolidWorks Custom Properties.  Third activate the revision automation feature within the PDMWork’s VaultAdmin tool.  Of course, this will require Vault Administrator access to the VaultAdmin. The setting is found under the Revision Table tab in the General section, called “Enable Revision Table”.

Once these three items are set up, drawings will automatically revise upon check in, with updated revision and title blocks.  Control over what appears in the added revision row is within the check-in screen itself when the drawing is checked in.  Further controls can be set up to limit or automate the value for revisions so that no mistakes can be made regarding the revision level of the check-in.  Within the VaultAdmin, there is even the ability to control the number of revisions visible on a drawing.  Utilizing this set up can save substantial time and eliminate potential check-in revision identification errors.