December 7, 2016, New Mexico SolidWorks User Group Meeting

Version 1

    This is the first meeting at our new location

    We have (hopefully) found a new long-term home at the HB & Lucille Horn Family YMCA, Teen & Technology Center (Downstairs). 4901 Indian School Road NE, Albuquerque, NM 87110.

    As before, we welcome any feedback you have about the new location (positive or negative).

    Our next meeting will probably be the second week of February due to SWW 2017 taking place the first part of Feb. 


    AGENDA

    Tom Cote (Applied CAD Solutions)

    Tom has been on CAD since 1983 and a CAD Admin since 87. He’s been using SOLIDWORKS since 1996 and a SOLIDWORKS CAD Admin since 97. He has extensive CAD & Data Management experience including implementing PDM as well as data migration for both large & small companies. Tom is very active in the SOLIDWORKS community and is the Co-Chair of the Central MA SOLIDWORKS User Group (CMA-SWUG) as well as the VP of the Boston Area North SOLIDWORKS User Group (BANSWUG).


    Neil Custard (3D iDesign, Inc.)

    Neil has used SolidWorks since its beginnings in 1997 and is one of the fastest 3D modelers on the planet having earned 1st place in the SolidWorks World 2012 Model Mania contest in San Diego, CA. as well as placing 2nd in 2008 and 3rd in 2010.

     

    Total attendees 43

    NMSUG First Timers 10

    Students 2

    SolidWorks Certified Users 12

    Planning on attending SWW 2017  3

     

    MEETING LOGISTICS - Ever wonder how we share valuable content, bring in out-of-town presenters and feed everyone at no cost to you? SolidWorks corporate places such high value on the user-group community that they reimburse all our costs. We pay for the meeting space and food up front and turn our receipts into the SolidWorks User Group Coordinator. We try to offer variety when it comes to eats. This time around, we had Sadie’s New Mexico Green Chile Stew, beans, rice, tortillas and biscochitos. Separately, Neil Custard’s travel expenses were also covered by SolidWorks.

     

    TONIGHT’S MEETING – SOME BACKGROUND INFORMATION

    Tom Cote’s presentation, broadcast live via the internet from the Holiday Inn in Boxborough, MA was part of the SolidWorks Largest User Group Meeting Ever or SLUGME. Todd Blacksher, President of SwugOne (SolidWorks User Group of Nebraska) and past presenter here in Albuquerque, was the instigator behind SLUGME. The meeting itself was hosted by the Boston Area North and Central Massachussetts user groups. Estimates are that thirty or more user groups tuned into the internet feed for Tom Cote’s presentation. At the time of this recap (five days later) there were 740 verified “attendees” with the numbers still coming in.

     

    Prior to Tom Cote’s presentation, surprise guest and SolidWorks CEO Gian Paulo Bassi opened with some introductory comments which are summarized here. Currently, the number of worldwide SolidWorks seats stands at about 3.5 million. Gian said 87% of the top universities in the world use SolidWorks. Graduating students who used SolidWorks in college find it easier to get jobs. SolidWorks education is embarking on an earnest effort to offer SolidWorks to students in high school and even in Jr. high schools.

    Tom Cote – Managing & Best Practices for Large Assembly Models

    After his brief comments, Gian turned the meeting over to Tom Cote-Applied CAD Solutions for his well-attended SolidWorks World presentation, Managing & Best Practices for Large Assembly Models. If you find that this is a long and boring read (I take no offense), jump down to the bottom of this section get the link to Tom's presentation slides. They will probably be easier to follow.

     

    What are large assemblies?

    What affects Performance?

    Using Subassemblies

    Configurations

    Display States

    Freeze Bar

     

    What is a large Assembly? If your assembly is slow to open, slow to regen, has choppy rotation, crashes, or you get system resources running low messages, then you probably have a large assembly.

     

    “I DON’T CARE, JUST MAKE IT WORK FASTER” commonly heard undercurrent when Tom is called upon to consult with clients.

     

    What Affect’s Performance?

    File Size-Level of detail

    Component rebuild times

    Complex geometry which can be further defined by face count and number of graphics triangles.

    How any parts (models) in top-level assembly: are there too many, can you create some smaller subassemblies?

     

    Here are some SolidWorks settings that commonly slow down large assemblies.

    Too many Reference Paths

    Models in an older version of SolidWorks-SWX converts old version parts every time you open that assembly

    Mate, rebuild and equation errors

    “Advanced” mates-they are cool but…

    Missing components

    Computer hardware-Keep video drivers current-not your video card’s latest driver, but the latest SolidWorks approved driver.

    How “clean” is your computer; cookies, do you have iTunes? Dust out your desktop workstation (reduces heat) from time-to-time. Once in a while clean out the backup files.

     

    HOW TO MEASURE PERFORMANCE

    Overall file size

    Individual model rebuild times.

    Use the Assembly Expert (pre-2016) or Performance Evaluation (2016 forward)

     

    SLOW PERFORMANCE-Too Much Detail

    McMaster-Carr screws are all built with equations. This results in a 40-50% hit in rebuild time depending on file size. Tom deleted the helical thread features and letters on the screw head and saved significant rebuild times. This also drops file size significantly.

     

    He showed a heat sink with all the fins and fillets shown. He reduced the detail and got the rebuild time from .59 seconds to .05 seconds and reduced file size by 75%

     

    Don’t model text. It kills performance. Emboss vs. Engrave? They are both the same. He tried the split-line method and the rebuild times got worse. There is yet a better method. Use the stick font method and the rebuild time goes way down. There is a font called OLFSimpleSansOC. If all the machine shop wants is a line for the tool cutter, this may work. It is a sketch so you would need to turn it on in drawings. File size goes way down.

     

    PERFORMANCE EVALUATION – Check it out, it tells you if you are running large assembly mode and lightweight mode.

     

    ASSEMBLY VISUALIZATION answers the question, what is your graphical performance hit? It measures rebuild times, graphics triangles and face count.

     

    Tom showed an add-on that looks at your files and compiles face count and triangles into an Excel spreadsheet.

     

    He showed a heat sink model where he reduced the number of faces from 450-22 and the number of graphics triangles from 1728 down to 268.

     

    He had another example with text on a face. Engraved text had 171 faces, split line text resulted in 26 faces but the stick font technique resulted in only 6 faces.

     

    SO ONCE YOU EVALUATE IT, HOW DO YOU FIX IT?

     

    Look for In-context circular references

    Look for files in older SolidWorks versions

    Fix all mate and rebuild errors

    Fix all equation errors.

    Pay attention to the reference paths that are set up on your system.

    Don’t work over a network. Work local and use check-in check-out.

    Fully constrain sketches. This does not make for a faster model but it decreases the chance of breakage. Same for assemblies, every item in the assembly is constrained.

    Ctrl-Q rebuilds the entire tree, Ctrl-B only rebuilds what’s been changed. Ctrl-B is faster.

     

    Limit how many parts or subassemblies are in the top level assembly: try to stay below 100 files and/or 300 mates. (Concentric/lock mate counts as one). This is just a rule of thumb but in his 30 years of cad admin, it has held true.

     

    Model threads ONLY for 3D printing…use configs. Have a simple config.

     

    Regarding video cards and drives, you only need a high-end graphics card only if you use Real View graphics or photo rendering in your daily workflow. The reality is generating graphics PAN, ZOOM and rotate are mostly CPU driven. Might invest more money in the faster CPU.

     

    SolidWorks Add-Ins are great if you use them. Be sure the keep off the ones you don’t use.

     

    System Option: Show thumbnail graphics in Windows Explorer, use this locally but not in a vault.

     

    System Option: Show latest news feeds in task pane…turn this off.

     

    System Option: Purge cached configuration data speeds changing configurations.

     

    Image Quality: Low is faster but most screws from McMaster-Carr come in at the high end. The location of the slider bar affects the number of triangles AND this increases the number of triangles. There is a checkbox that allows you to apply your image quality settings to all-referenced part documents.

     

    Check the box that says “Use large assembly mode” IT WORKS, use it. Tom sets it at 500 parts.

     

    Referenced Documents (Under file locations)-it goes these locations in order until it finds the part. These are the paths it uses after checking in the RAM. You can toggle this off.

     

    Freeze Bar-Read up on the freeze bar. It causes a minor improvement in file open times, 5%. Tom personally likes to freeze all parts released to production. Rebuild time for frozen parts is 0.

     

    If you have to have the detail, use simplified configurations. Tom makes them derived in the part model and the assembly model. He likes to have the detail in the top level assembly but simplified in subassemblies.

     

    Build a simplified derived configuration in your start parts (assembly models).

    The simplified top-level assembly should reference all the simplified component configurations.

    Suppress internal (not seen) components in the assembly model.

     

    At 150 to 200 mates, it’s time to start thinking about file structure and adding another layer of subassemblies.

     

    Subassemblies do not have to rebuild all their components and mates when the parent assembly rebuilds.

     

    Advanced mates give a pretty big performance hit. Flexible assemblies are the worst.

     

    It is good modeling practice to put fillet and chamfers at the bottom of your tree. It’s easier to turn on and off. Don’t mate to them.

     

    Tom Cote has graciously made his presentation slides available in a 60 page pdf. The document is available here: https://forum.solidworks.com/docs/DOC-3471

     

    NEIL CUSTARD - SolidWorks Tips You Need to Know

    Neil runs the website SolidWorks tips daily. He has worked as a trainer for GoEngineer, Aerospace Design Engineer 8+ Years. Model Mania winner three times, owned 3D iDesign, Inc. Neil’s vast experience includes new and updated design, reverse engineering, implementations of standards, SolidWorks and PDM Installation and Training and Best Practices Implementations.

     

    Neil currently owns and operates solidworkstips.com and 3D iDesign.

     

    Over the years at SolidWorks World, he has taken 1st, 2nd and 3rd in Model Mania competitions.

     

    For his presentation, Neil presented us with a game of SolidWorks Jeopardy. The game board had four categories: Parts, Assemblies, Drawings and Potpourri each with options for 100, 200, 300, 400, and 500 points.

     

    Parts for 200 - Creating a part with this tool allows for the correct drawing and dimensioning or 2nd operation drawing without the need for previous dims. To create a machine drawing for a casting use INSERT PART-Solid Bodies. Bring in that model and it is a reference. Neil likes insert model items-dimensions, especially those with tolerances. They get changed in the part file and update on the drawings.

     

    Potpourri for 200 - This sheet metal tool will create two bends in the middle of a part based on the cutout length-WHAT IS THE JOG TOOL. Use a surface, cut with thickened surface. Draw a single solid line sketch somewhere in your cutout and only on the part that bends. Then use the jog tool. This is a cool tool, probably not used much.

     

    Drawings for 400 - You can view more than one sheet of a drawing by doing this? Use the standard windows NEW WINDOW command. Test this on a dummy part to see what happens when you save.

     

    Assemblies for 300 - This assembly tool will allow you to pattern your parts based on a pattern. What is a PATTERN DRIVEN PATTERN. Neil modeled a disk brake rotor with a hole pattern in it. Using Pattern Driven Pattern reduces mate count often times significantly (with a fastener stack up) for example.

     

    Potpourri for 300 - This is a quick way of simultaneously changing all or most of the drawing view configurations. SHIFT CLICK FROM THE DRAWING FMT. Shift click the drawing views also.

     

    Parts for 500 - Using this tool will allow you to only shell part of your model without having to reorder features? WHAT IS A SPLIT PART? (Stick Shift example). The split part tool uses surfaces, planes and lines to split a part. Now you can shell just one of the split bodies. When finished, you can combine them if you want.

     

    Parts for 100 - With this automatically given tool from SolidWorks you can almost totally eliminate creating reference geometry axes in your FMT. WHAT ARE TEMPORARY AXES?

     

    Weldments for 400 - When creating a bent tube in a weldment clicking on this wall will allow you to connect two tubes together. What is MERGE ARC SEGMENT BODIES. This technique can be used to control cut-list behavior.

     

    Assemblies for 400 - How to animate a spring? What is TWIST ALONG PATH. Build a spring in the context of an assembly. Use a circle, make a sweep, use guide curves, specify twist control value, 5 revolutions. Then animate it.

     

    Drawings for 500 - Showing hidden lines in a drawing view. What if you want to show just some of the hidden lines in a drawing view or maybe just the hidden line for one part of an assembly? DRAWING VIEW PROPERTIES > SHOW HIDDEN EDGES TAB where you can select the part and see the preview OR you can just choose the feature from the FMT from within the part.

     

     

    “Neilisms”: Neil made some interesting comments that force us to think about our modeling techniques. (These are AWESOME, thanks for catching these!)

     

    The more relations in a sketch, the slower your model. A dimension is a relation.

     

    If you don’t need the dimension on the drawing, then you don’t need it in your model.

     

    Neil prefers to stay away from sketch patterns as much as possible (more relations) and confusing to customers.

     

    In most cases, within an assembly, linear and component patterns should not be used. They can nearly always be driven by another pattern.

     

    Neil uses lots of hybrid multi-body modeling.

     

    Use temporary axes almost always in lieu or a reference geometry axis.