Solid Modeling Blog

Solid Modeling at PVEng

Some quick notes on getting the most out of SolidWorks.

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Making Repads Using Offset Surfaces

PVE-7253, Last Updated Nov 27 2015, By: Cameron Moore, Jordan Winger and Laurence Brundrett

Yet another repad modelling method, this one for more difficult designs where the previous two methods presented below will not work. The repad can be built onto complex surfaces. Developed by Jordan Winger of Hawk Ridge Systems, shown here with a few minor changes.


The finished product – a branch connection covering a swept feature with more than one radius, welds are not shown.


The start of the development: A flanged and dished head has a straight flange, a knuckle radius and crown radius. Normally when swept 3 different surfaces are created. These 3 surfaces lines are combined to create 1 fit spline.


This is important – once revolved, the fit spline creates a solid head with only one outer and one inner surface. This allows the repad to extend beyond the limit of the crown onto the knuckle and if required onto the shell as well.


A nozzle is extruded onto the head, it is not merged. No hole is cut yet.


A circle radius of the desired repad size provides the profile, and the end of the nozzle provides the path for a sweep. The radius of the profile provides a distance to the limit of the repad, not the true developed width of the repad which is larger due to the curvature.


The top surface of the head is duplicated.


A line at the intersection of the swept shape and the duplicated top surface defines the limits of the repad.


The duplicated top surface is trimmed to the intersection line.




…inside cut and combined for the finish!

Making Repads Using the Flex Command

PVE-7253, Last Updated Nov 26 2015, By: Cameron Moore and Laurence Brundrett

Here is another method of making repads, this time using the Flex command. When this method works, it is simpler than using surface commands. This method developed by Cameron Moore is particularly useful because it creates a properly contoured repad that can be used for a Drawing or for Finite Element Analysis.


The finished product – a branch connection complete with repad – welds are not shown.


The start of the development: two solid parts – 1) the header and 2) OD and thickness of the final repad. The Repad is drawn on a plane tangent to the OD of the header.


This is the magic – the repad is flexed to match the OD of the header. The repad edge is perpendicular to the Header the whole way around.


The branch is extruded from a new plane at the end of its extent, down to the repad. The extrusion command merges the header, repad and branch.


Finally the branch hole is cut finishing the model. Welds can be added – there are no gaps for easier FEA analysis.

Automated Drawings – Productivity and Quality

PVE-6322, Last Updated: July 29, 2013, By: Laurence Brundrett

I have long had two interests in data links between calculation packages and drawing packages: 1) drawing quality; and 2) drawing productivity. I have worked on spreadsheets that produce DXF drawings directly, transferred data directly from Excel to AutoCAD to create flat layouts of complex sections, modified SolidWorks shapes from Excel and most recently attempted to get drawing data to transfer directly from programs like PVElite into AutoCAD.

The quality issue is obvious. Any number that is first entered in a calculation program, and re-entered into a drawing package is subject to error. Not only do the numbers have to match, they have to keep matching through all design revisions. The productivity issue involved with the necessary re-entering and checking is obvious as well.

Pressure vessel calculation packages have long been able to make drawings, but they were not very impressive, and I know of no company that actually used them. Codeware has released a package for their Compress program that I think starts to overcome the issues with computer generated packages. They call it “Inspect”. It works inside Compress to export data, and inside SolidWorks or Inventor to convert the data in usable imported solids.

Codeware Interface

The program is in development, but I find that the results are usable right now. I took one of our sample jobs done in Compress (Vertical Vessel) and used Codeware Interface to export it to SolidWorks. With very little effort I had a solid model and a the start of a drawing with Bill of Material, all with no data re-entry.

AutomaticDrawingBOMYes this is preliminary, no it does not update easily as the design is revised, but Codeware is still developing it. If it can get to the point where calculation changes show up in the model or the other way around, then it could be very useful.

Making Size on Size Branch Connections with Repads

PVE-7253, Last Updated: July 29, 2013, By: Cameron Moore and Laurence Brundrett

Modeling size on size connections with repads can be difficult. This method developed by Cameron Moore here at PVEng is particularly useful because it creates a properly contoured repad that can be used for a Drawing or for Finite Element Analysis.


The finished product – a size on size branch connection complete with repad – welds are not shown


The start of the development: two surface parts – 1) the OD of the branch and 2) the OD of the Repad on the Header are developed.


This is what makes this method work so well – the repad outer surface is trimmed to the OD of the branch pipe…


… and extended an equal amount all the way around. Note that the repad is bent under itself as it goes around the branch pipe. A projected cut from the branch onto of the OD of the repad would not work.


Thickening the repad converts it from a surface to a solid. Note that the edges are perpendicular – a feature that cannot be obtained by using projected cuts.


A solid header has been created and the surface branch has been replaced by solid pipe. Here shown in section view.


An opening in the header for the branch completes the model unless repad and header fillet welds are also required…


… addition of the welds.


The solid model made this way is without gaps making for easy FEA analysis!

Things That Cannot Go Wrong!

PVE-6322, Last Updated: July 29 2013 By: Laurence Brundrett

Solid Model Sketch of Flanged and Dished Vessel Head

A Flanged and Dished Head

The sketch that creates this flanged and dished pressure vessel head has 6 dimensions that need to be updated before it can be used:

  • OD – outside diameter (85.750″)
  • tNom – Nominal Thickness(0.750″)
  • tMin – Minimum thickness after forming (0.625″)
  • SF – Straight Flange(2.000″)
  • ICR – Inside Crown Radius(85.750″)
  • IKR – Inside Knuckle Radius(8.000″)

These dimensions are taken from the calculation set which is run first. Normally, the user has to set these dimensions three times: first in the calculation set; second in the parts sketch and: third for the part description that shows up in the Bill of Material. These three sets of dimensions must be kept in sync no matter how many times the design is revised!

Solid Model Sketch with Dimensions

The required dimensions to create a Flanged and Dished Head

This part from our library builds it’s own description. The custom properties for the part has an entry for “Description” that contains a long formula:

Head, F&D – “OD@Sk1@F&D Head.SLDPRT” OD, “tNom@sk1@F&D Head.SLDPRT” Nom., “tMAF@Sk1@F&D Head.SLDPRT” MAF, “SF@Sk1@F&D Head.SLDPRT” SF, “ICR@Sk1@F&D Head.SLDPRT” ICR, “IKR@Sk1@F&D Head.SLDPRT” IKR

F&D Head.SLDPRT is the files name. SolidWorks reads the dimensions from the model and populates the description:

Head, F&D – 85.75 OD, .750 Nom., .625 MAF, 2.000 SF, 85.750 ICR, 8,000 IKR

This complete purchasing description always matches the dimensions in the model no matter how many times it is updated! A source of errors has been eliminated and the amount of work reduced. If only there was some way of automatically linking the model dimensions to the calculation set…

Postscript: See Automated Drawings – Productivity and Quality above for advancements in the effort to link drawings to the programs that generates their data.

The Joy of Weldments

PVE-5804, Last Updated: Aug. 21, 2012, By: LRB

Solid Model of Spherical Pressure Vessel

Intermediate stair landing for a storage sphere

The SolidWorks weldment toolbox can make it easier to create complex assemblies. This intermediate stair landing for a storage sphere consists of 26 pieces. I have two versions of this assembly. This first is built as an assembly of 15 separate parts. It was hard to build and each part had to be mated in an assembly. Updates for different sizes of storage spheres was difficult.

Solid Model of Stairway Landing

Final results as a weldment

The second version is built as one part in a weldment. 15 part files and 1 assembly are reduced down to 1 part file. The design is based on one 3D master sketch.

Sketch of Stairway Landing with Dimensions

A bit messy but good – the master sketch

The master sketch is a bit messy, but design changes are quick and easy. The time required to make the weldment was less than the time required to make the assembled version. The file is also 1/3 the size and loads much faster – very important when dealing with an assembly with multiple parts like this.

Bloating SolidWorks Files

File: File:PVE-4482, Last Updated: Aug 18 2010, By: LB

This SolidWorks part for a weld neck flange has a design table with 132 different configurations in it. The configurations cover changes in size and rated pressure. When the file was first created it was 2,422 KB in size (2.4 MB). With use it has grown in size without any changes to the file.

B16.5 RFWN Flange

A configurable model of a standard flange

Design Table

The design table has 132 configurations:

B16.5 RFWN Flange

File Sizes as the file is used

The original file was 2.4 Mb in size. Each time a different configuration is viewed, the file size expands when it is saved. When all 132 configurations have been viewed, the file has bloated to 68.5 MB. The file has to be saved, closed, re-opened and saved as (without viewing additional configurations) to get it back to the original 2.4 MB size.

I have been told and I have no way of knowing if it is true, that SolidWorks stores the surface display information for each configuration viewed. If this is true, then the files would be made larger to prevent the requirement to re-generate the surface information when viewed. The save – close – re-open – save-as restores the original file size by removing the surface information for each viewed configuration.