After posting this last week I had a discussion (via Twitter) with Vajrang Parvate – Director Product Development – Dassault Systemes SolidWorks
As you can see there was the question in regards to where I was taking my file sizes from. The simple answer was what I could see on the disc. Vajrang generously offered to look at the files and educate me (the latter not always that easy!) So here is the educating part. The file size we see on the disc is more than just the “model” size (the raw data) it comes with “overhead”. That can vary depending on how the file is saved (Save v Save As) or where (local disc v network drive), the type of data and the list goes on! (I can see a whole other post in this!)
It’s a good thing that Vajrang did have a look. The “raw data” file size on average was around 5% less in size than the “size on disc” for all but one! It appears that my methodology was pretty good but not perfect. It hasn’t had a big effect on the observations between Features V Sketches BUT I have corrected and updated below and I have apologised to Sketch Fillets.
So what about the PLUS he mentioned!
If you think the SolidWorks Development team isn’t putting in the effort THINK AGAIN! Not only did Vajrang run the files through SolidWorks 2014 he also opened, rebuilt and Saved in SolidWorks 2015 Alpha 1. So here’s a “World Exclusive” (always wanted to say that) on average the file size (seen on the disc) for most of the files was around 40 to 50% smaller than the SW2014 files!
Just another reason to look forward to seeing SolidWorks 2015
I must Thank Vajrang for checking the files, pointing out my error and sharing some knowledge. I greatly appreciate it
Over the past few weeks I’ve been starting to record opening times for a few of our main Assemblies. There were a few reasons for this. First we had made the decision to change anti-virus programs and I was interested to see what difference this would achieve. I also wanted to make the case for a new computer. Finally I was having a few discussions about Large SolidWorks Assemblies.
The outcome of this has been that we have seen a decrease of around 19% in opening times by going to a “web base” anti-virus (Webroot) I didn’t need to make the case for a new computer as I was told the other day that I should put together a specification for what we need! As for the discussions about Large Assemblies, well that has lead on to a discussion about good CAD modeling techniques and how that effect computer performance!
There is often talk about “Rules for good Solid Modeling” and what constitutes good CAD modeling techniques and why it is important. Much of that discussion normally revolves around preventing problems when making changes at later stages. Either with issues of “Parent-Child” relations or simply making life easier for others when they are looking to make those changes!
I thought I should have a look at a few of those “Rules” in the context of what effect they would have in regards to computer performance
Relations V Dimensions
Use as many relations as you can to control the sketch over the use of dimensions. Most times this will be simpler and faster. The bonus is a much reduced file size. The following is a simple two feature part.
Features V Sketches
It is better to use Features instead of Sketches. I’m certainly guilty of not doing that! I’ve always been one to use sketch fillets.
I was not aware of the effect until I had this look at them!
There is not a big difference in file size between using sketch fillets and using Features Fillets. The sketch fillet files is 5% smaller however it is the rebuild time where we see the biggest difference with sketch fillets increased by 43%
Single Sketch V Sketch Per Feature
I’ve never been one to use a single sketch and the Contour selection with the Feature! There is something I just don’t like about the look of it! It’s a widely promoted technique shown to be a fast way of doing things! I see it ever year at SolidWorks World with the Model Mania competition! So it was interesting and somewhat surprising when I saw the results
Cut Extrude V Hole Wizard
Over the years I have swung back and forth between using Cut Extrude and the Hole Wizard for the screw holes in our cabinet parts. Currently I’m back using Cut Extrude!
This was an interesting results. There is not a lot in it. A small 2% increase in file size and a sizable 27% increase in rebuild time. However there is a caveat. I don’t need to produce drawing for the cabinet part. Simply export dxf for our CNC Router. Hole Wizard allows Hole Tables and call-outs in Drawing. Right tool for for the right job!
Fillets Towards the End
I’ve been guilty more times than not of using Fillets as I go. Certainly it can have effects with Parent – Child Features and I need to make a far more conscious effort in that regards. I was somewhat surprised with the results. I guess I was expecting a bigger increase in rebuild times
Now that I’m starting to understand Surface Features I’ve been reassessing how I produce some parts. It was a good opportunity to see what effect it may have!
Surface Features V Solid Features
A simple model created with a Surface Loft and Thicken compared to a Solid Loft and a Shell
The Surface model had a very small saving of 4% in file size but a some what surprising 54% increase in rebuild time. However what was more interesting was that on both models most of the rebuild time was in a Full Round Fillet!
So I had to look to see if there was an exception to every rule! Sometimes Sketches are better than Features! A sketch with a tangent arc, a revolve features will sometimes be better than a Full Round Fillet! As this simple model shows!
Whilst I’m a great believer in the “philosophy” of Colin Chapman innovating Engineer and founder of Lotus Cars who said “Rules are made for the interpretation of wise men and the obedience of fools” There are at time good reasons to follow the accepted good practice!