Building Big Boms - Continued more

Continuing on from the previous 2 articles on this matter, using SolidWORKS procedures to Build Big BOM's using multi-bodied part techniques.................

MULTI-BODIED MODELLING TECHNIQUES

SolidWORKS is designed to use multi-bodied parts. It specifically and uniquely uses a ‘Part environment’ for it’s Frame Work / Weldment generator.

The advantage of Weldments is that you can create a Weldment Fabrication cantaining multiple Steel Sections / Plates and manage the separate parts and their relationships with-in the one file, without the need of any external references, external Links or separate files etc.

The weldment tools within SolidWORKS also include the functionality to include Sub-Weldments with-in the one file. SolidWORKS, also has the power, to insert library part files into your Weldment Fabrication. (Insert a Part into a Part and ‘constrain’ like an assembly) using the ‘copy, rotate and move’ tool. Some of this functionality can be found on the SolidWORKS Online ‘HELP’ documentation.

https://help.solidworks.com/2018/english/SolidWorks/sldworks/HelpViewerDS.aspx?version=2018&prod=SolidWorks&lang=english&path=sldworks%2fc_Multibody_Parts_folder.htm&id=5ad6592048e142e2a34423437ce79a44

 https://help.solidworks.com/2018/english/SolidWorks/sldworks/HelpViewerDS.aspx?version=2018&prod=SolidWorks&lang=english&path=sldworks%2fc_Multibody_Parts_folder.htm&id=5ad6592048e142e2a34423437ce79a44

 

Expanding this philosophy further, using similar modelling techniques, I propose that relative steel work (or where ever else that is appropriate) with bolt-on ‘Sub-Weldments’ can be developed in one ‘Multi-Bodied’ Part file. This can be very successful on ‘Groups’ or ‘Units’ of Structural Steel Assemblies. E.g. this CST Lifting Frame.  

As with most things there is a balance of Pro’s and Con’s associated with this modelling practice.

Advantages include;

1. All parts contained in one file.
2. No external references (Except for any Library Parts inserted)
3. Mating parts or aligning holes can use the same planes, sketches or features (e.g. Extrude Cut) without resorting to adaptive (externally linked) features.
4. Can be used as a simplified ‘Part’ for ‘Building Big BOM’s’ procedures.
5. Easily can ‘save as’ new part and modify Length, Width, Height etc. without the need of PDM Works, SolidWORKS explorer or manually locate external files / Links, to make similar versions etc.
6. No Need to create part numbers of individual ‘Parts’ until your design is completed and the parts are designed appropriately etc.
7. No need to develop Sub-Assemblies or Sub-Weldments in advance. (Can break out into Sub-Assemblies / Fabrications once engineering been completed.)
8. Can create Engineering Drawing using Cut-List and detailing Multi-Bodied Part before exporting into Split Assembly. 

Disadvantages include

1. Additional Data Entry in your part file. (i.e. typing in Part numbers and naming each instance of each part number manually)
2. Additional training and procedure development required.
3. Configuration grouping in your BOM on your Drawing to ‘Group’ the instances of each multi-bodied Part. (To get the quantities correct of each part)

The bodies are automatically named and uniquely numbered based on the last feature used to create them. In this example Boss-Extrude56 & Boss-Extrude57 was used to create 8 different ‘bodies’ of the same part.   

These bodies can be grouped easily into different ‘part’ numbers by creating an automatic cut-list. This is literally completed by clicking your mouse on a check box. The automatic cut-list is like Windows Explorer folders. They contain all the ‘like’ bodies. The folder names are automatically generated and become the ‘Part’ number.

To issue these company designated part numbers, you are required to manually input data (unless your ‘Part Numbering’ issuing system preforms Macros and interrogates the meta data internal to the SolidWorks program) and works just like renaming Windows Explorer folders.

In this example, as we have not yet decided to move forward on our ‘Part Numbering’ system and continue just to use ‘Item Numbers’, and for ease of not wasting unnecessary time generating numbers in the current database which won’t be used, I have used ‘Dashed’ numbers of my original ‘Part’.

As you can ascertain, from the left image, there are currently 104 ‘bodies’ split into 22 ‘Part Numbers’, including P7428 which is a purchase part of the Rud Lugs.

 

Split Assemblies

 Multi-Body Parts and not dynamic. As a result, they have some disadvantages and, in some cases, to eliminate these disadvantages it is beneficial to create a Split Assembly.

 The disadvantages which can be eliminated by creating a split assembly include;

1. Move Components – free move (without using Move, copy & rotate command)
2. Dynamic Clearance
3. Collision Detection
4. Advanced mating (including driving, cam and other motion circumstances)
5. Create Sub-Assembly / Sub weldments / Fabrications without corrupting the Weldment Cut-List.
6. Building Big BOM’s performance

More information can be found on the online SolidWORKS help link below.

https://help.solidworks.com/2018/english/SolidWorks/sldworks/c_Multibody_Parts_Vs_Assemblies.htm?id=90846a79e64b4d6a8db3fe4e67abd529#Pg0

 In this example, CST Lifting Frame, we have 2 reasons to create a Split Assembly from our Multi-Bodied Part. Advanced Mating, (Driving the Frame with Hydraulic Cylinders) and breaking out our design into Sub-Weldments / Fabrications

So, as previously documented, a disadvantage of creating a ’Split’ assembly is extra ‘data entry’ and ‘procedural development’. 

Naming each instance of each ‘Part’ with a unique number is the extra ‘data entry’ required. I usually adopt the approach of putting a letter after the part number or if there are more than 26 bodies of a specific body I put 2 letters as a suffix. (As shown )

 

The procedural requirements required in a ‘split’ assembly include

1. Exporting and managing the bodies to external files.
2. Creating Sub-Assembly or Sub-Weldments / Fabrications using these external files.
3. Adding / Editing amendments as required.

The ‘Split’ Assembly file name will be the same as the original Multi-Bodied Part file name. (with a different ‘Windows’ extension) The original file name was M4003.SLDPRT and the ‘Split’ Assembly will be M4003.sldasm.

Split Assembly.

Our ‘Split’ Assembly has the same 104 bodies, now saved (with the same name as the body it refers to) as individual parts, which have a single ‘derived feature’ in the feature tree linking the part back to the original Multi-Bodied Part. All these parts are fixed in space (with no mates or constrains) about the same origin as the original Multi-Bodied Part.

Now we have an assembly file we can start generating our sub-weldments / fabrications. These will be external files as well and numbered as per company’s policy. They need to ‘ground and rooted’ (fixed to the origin) into our ‘split’ assembly. These Sub-Assemblies may also need a Suffix to accommodate the same Fabrication with a Quantity of more than 1 off. (Don’t get bogged down with these suffixes, there are procedures to exclude this from the BOM on the drawing to get the Quantities correct on the drawing.) 

 Split Part

Now we just drag our ‘Split’ parts into the correct assembly. Leaving them ‘Ground and Rooted’

Notice how all the parts, assemblies etc. all have the same origin, have no Mates / constraints and are all fixed?

 Once you have all your Sub-Weldments / Fabrications sorted into your desired ‘part numbers’, (by dragging all the ‘split’ parts into the correctly named assembly file, with suffixes if required) you can start adding the required parameters / properties into the files.

 Please Note: It is also beneficial to place individual parts (e.g. Brace Members) into an assembly file.

Now let’s look at getting the BOM right on our drawing and the process required to remove the Suffixes from your part numbers and group the same parts to enable the BOM quantities to be correct.

 

When you drop a BOM into your drawing, depending on your template and setup etc., the ‘Configurations\Part Configuration Grouping’ setting is normally set to ‘Display configurations of the same part as separate items’. If this is not the case than this must be selected when you first drop in your BOM in your drawing. (or if not, you can change this property after the BOM creation in the BOM properties.)

To really get to know this procedure, I have selected to examine the Angle Bracing more closely.

Due to being created from a ‘Multi-Bodied’ Part all these files have a Suffix after the ‘Part Number’ which we don’t wish to exist to the Drawing BOM.

Below Figure shows which bracing we are going to investigate further.

 

 In our ‘Split’ Assembly there is 4 off M4070 assemblies, each with a different suffix. As shown Below.

With the Correct Setting selected in the BOM as detailed above, the Drawing BOM will list these Parts as 4 different lines. As shown Below. This is not the desired Outcome. We actually want the BOM to say 4 off M4070 and ignore the suffixes.

When we open the Bracing File and look at ‘configuration’ properties this is what we find as default. See Right Image.

So, looking at our BOM which we placed on our Drawing, when we click in the ‘Part Number’ Box of each line, we have the option to delete the suffix.

So, if we edit all the lines and remove all the suffixes from the ‘Part Number’ in our drawing BOM what does this do and how does it effect the properties in our ‘Model’?

 Ungrouped BOM with Suffix Removed

So, you can see all the Suffixes have been removed, however, the ‘like’ parts still haven’t been grouped. Before we look at how to group these ‘like’ parts lets look at how removing the ‘Suffix’ from the Drawing BOM has affected our ‘Model’?

 All that has happened, and you can change it back or edit the option in the parts before creating the drawing, (Although, removing the Suffixes from the Drawing BOM is the quickest easiest way of achieving this) is the ‘Bill Of Materials Options’ in the configuration properties has changed from ‘Document Name’, to ‘User specified’

Now if you go back to our Drawing BOM property dialogue Box and change the ‘Configuration\Part Configuration Grouping’ setting to Display configuration with the same name as one item number our BOM will read how we would expect.

 

 

 

 

 

 

 

 

 

 

 

 

 

 Note: Quantities are right, and Suffixes are not shown.

1.2.   Building Big BOM’s

Building Assemblies in SolidWORKS (or any parametric software) requires planning, especially when you are building substantial assemblies, which have many levels and include Sub-Assemblies, Weldments / Fabrications, Sub-Weldments / Fabrications, Fasteners, complex mechanical arrangements and full manufacture details.

 People are sold on the dream of parametric software; however, the dream soon turns into a nightmare when the model gets out of control and becomes unmanageable.

 There are generally many reasons Assemblies can fall over and become to hard to manage, however, the main reasons I have found are by utilising tools designed for small assemblies as a quick & easy ‘cheats’ to get a model completed quickly.

 The features to avoid in SolidWORKS for large model stability and efficiencies are;

1. Adaptive Modelling
2. Top Level Skeleton Modelling
3. Projecting faces, edges or sketches in context of another part within an assembly.
4. Assembly Face to Face Constraining / Mating.
5. Obviously unavoidable in some instances however, main equipment and most major elements of your design should have local origins and should be positioned using either the default origin planes or user created planes for placement.
6. Assembly Patterning
7. Just place the objects into the assembly individually and constrain as required. (May initially take longer but is a good investment for model stability)
8. Assembly Mirror Components.
9. Manage Mirror Components at a ‘part level’ and drop in the correct version into the assembly.
10. Keep things Resolved
11. Avoid circular references
12. Incalculable equations
13. Insolvable Assembly mates
14. On a Part Level avoid bells and whistles like;
15. AutoCAD Direct Modelling tools like Move Face, Move/Copy Bodies, Split (Bodies), Combine (Bodies), Delete Face.
16. Feature Patterns
17. Rib, Draft, Shell and Wrap Features
18. Hole Wizards
19. Surfaces (in General)
20. Avoid Weldment Tools like; (utilise library sketch blocks)
21. Member creation,
22. Member Trim
23. Endcap etc.

 

1.2.1.  ‘Split’ Assemblies for BBB’s

 We have already looked at ‘Split’ Assemblies. Let’s look at expanding this knowledge to enhance our modelling capacity to help efficiencies in Building Big BOM’s.

First thing I want to look at is utilising ‘Library Sketch Blocks’ in our Multi-Bodied Part instead of the default ‘Weldment Member’ Tool to create our Hot Rolled Steel Members.

Sketch Blocks for Hot Rolled Sections.

Notice how the radius are not included in the sketch blocks? The more faces and curves etc. in your model the less efficiencies you have. By removing these radiuses in your sketch, you create an opportunity to increase performance of your Big BOM model.

Our Multi-Bodied Part Doesn’t have Radius on the PFC Members or on the Gusset Plates. This is because this Multi-Bodied Part becomes a simplified part by default and is the actual model which is placed in our large assembly to increase performance.

 

All the details go into our ‘Split’ Assembly, including, Sub-Weldments / Fabrications, Fasteners (Bolts, Nuts & Washers) Sheet Metal Properties and radiuses etc. which is then used to detail this arrangement. The Split Assembly and all the ‘Split’ Parts remain linked to our simplified Multi-Bodied Part, so if changes are made to our Multi-Bodied part, they are reflected in the detail drawings and ‘Split’ Assembly.

 So, let’s look at how this works……………….

 Above is a ‘Split’ Part which has a derived feature which is the link to the ‘Master’ Multi-Bodied Part. The part is a PFC member without the internal Radiuses. Should we require for detailing or commercial reasons we can add a feature fillet to this part.

We can add extra details and features to the ‘Split’ Part to avoid clogging up the Multi-Bodied Part, which is going to used as a ‘simplified part’ in our building Big BOM’s efforts to populate our Top-Level Assembly to increase performance.

This step is not a requirement unless a need is identified to check clearances or create a cosmetically pleasing model for commercial purposes etc. However, let’s look at creating the Gusset plate to have the Radiuses and 1mm manufacture clearance for installation.

 

We can even create an offset sketch of 0.5mm to complete an extrude cut to add our manufacture tolerance on the laser cut plate.

 

Building Big BOMS requires careful planning and understanding of model practices. Using these Procedures, we have developed a Multi-Bodied Part which is simplified and an advanced model which we used for detailing. These models are linked and are update together.

 

The Advanced Model contains

1. Exploded Configurations for Detailing
2. Animations for driving positions of Hydraulic Cylinders, including positioning representations.
3. Sub-Fabrications / Weldments broken out into separate assembly files.
4. Fasteners (Bolts, Nuts and Washers)
5. Hydraulic Cylinders
6. Manufacturing Clearances and Tolerances
7. Full Fillets on PFC’s, Angles and gusset Plates
8. Phantom Assemblies for detailing Purposes
9. Material Properties etc. required for detailing.
10. Contains all the sheet metal and folding properties (if required)
11. Derived Features back to Master Part.

The Simplified Model is the ‘Master Part’ used to create the advanced model using derived features to the split parts. It has no Bells and / or Whistles and can be used in the upper assemblies to free up processing time and improve efficiencies.

1. Has no Fillets on any members. e.g. PFC, Angle or Even gusset plates etc.
2. Contains No Sub-Weldments / Fabrications or external files (except any Library Feature Parts inserted. i.e. Rud Lugs.)
3. Contains no Manufacturing Tolerances.
4. No animations or configurated explosions.
5. No Hydraulic Cylinders
6. No Fastening. (Bolts, Nuts or Washers)