We are quite new to SolidWorks and evolving standard practices for other users in your organisation.
I have a doubt about stock size and weight in BOM
Is there any way to show stock size and stock weight in BOM for the following coditions :
1. Cuboidal part with machining margin in stock
2. Cylindrical part with machining margin in stock
3. Multi-body part (plate weldment) with combination of above two.
How are you managing this (stock size and stock weight) in your BOM?
Thanks in advance.
We use 2 2d sketches that we drag to the bottom of the tree that have links back to a custom property size and also equations for the material weight. We add relations of the two sketches to the max width needed for stock size. This then will update if the part should change in size.
Thanks Mauricio and John.
Currently we are making a solid envelope in a new configuration (StockDefault) as per the shape of stock and deriving the sizes and weight from there. In this way equation is also not required, as equations fail to calculate weight for multiple cofigs. This is going well for single body part.
But the problem is for multibody part.
Is there any better way?
Vikas,
If you post a Zip file with a sample of the part (single or multi-body), will be a lot easier to show you how to do it.
Also, is there any particular reason to need muti-body parts? in reality, a multi-body part is something that do not exist, a part is a single solid, more that one solid is an assembly of parts (two or more solids). There a few instances where the use of multi-body parts is required to be able to model a component, however parts should be modeled as they are fabricated in the shop floor. In our case, we have modeled millions of components and only used multi-body parts no more that 10-14 times and that is only when due to "limitations" on SW we where unable to model the component the correct way.
Over 90% of the problems encountered with any CAD tool are caused by incorrect structure of the model or the modeling technic.
In reality there are multi-body parts called WELDMENTS.
In my view, starting from stock (as suggested by a few people https://forum.solidworks.com/message/90164#90164) and then doing operations similar to shop floor is not a good practice. Because finish/machined part is PRIMARY thing that you get from top-down approach and stock is SECONDARY which should depend on finish sizes.
Parts are attached here.
The multi-body part attached here is a simple one with only one configuration. But things can go more complex in some parts.
Vikas Garg wrote:
In reality there are multi-body parts called WELDMENTS.
In my view, starting from stock and then doing operations similar to shop floor is not a good practice. Because finish/machined part is PRIMARY thing that you get from top-down approach and stock is SECONDARY which should depend on finish sizes.
Parts are attached here.
The multi-body part attached here is a simple one with only one configuration. But things can go more complex in some parts.
Vikas,
I will take a look at your parts and see how you can obtain the dimensions and weight of the stock (blanks).
By the way WELDMENTS is a way inside SolidWorks of modeling ASSEMBLIES of INDIVIDUAL parts welded between them into a single "frame", representing them as a single part but having the ability to produce a BOM of individual components (a pseudo-assembly), but in reality (on the manufacturing process), it is an assembly of individual parts. When usign the WELDMENTS fucntionality you gain some and you loose some... in our case we produce (and therefore model in our CAD) products entirely made of steel profiles (structural shapes and large formed sheet metal parts) having very large size, complex structure and a large number of parts (in excess of 1000) grouped in many levels of sub-assemblyes, and we do not use WELDMENTS because of the limitations of this module for our type of work. However for some type of work we recongnize that it is a nice tool. One of the many limitations of this module is the inability to obtain detail data of each component of the assembly (weldment), another is that if you use formed profiles (formed sheet metal) you can not produce the flat patterns required to fabricate the profile, it is OK for frames build entirely with standard structural profiles since there all you need is the length of each member (the cutting list) and from that information you can get the rest (weight, etc.). Some other limitations have to do with the ability to perform optimization analysis using SW Simulation and with the limited ability to create 100% parametric assemblies. The advantage is that when it can be use, Weldments will allow you to produce the model faster that if you model using parts inside an assembly.
When I mention "model in the same way the product is fabricated" I do not mean you start with the Stock and then do the same operations as manufacturing to produce the model of the part... I was reffering to the way you should STRUCTURE the assembly, sub-assemblies, etc. not to the way you generate the solid of the finished parts
Hi Mauricio, have you found any solution for this.
Regards.
Vikas,
I have been outside my office on a couple of projects, as soon as I get some free time I will take a look at your files and see what I can do.
One way to do that is as follows:
- Create a 3D sketch representing your stock material (the envelope), this sketch can be related to the sketches defining the geometry of the part (the features).
- Place dimensions on the above mentined sketch (driven dimensions in case the sketch is related to other entities).
- Use ecuations to calculate weight or any other data you may need which can be calculated from the X,Y,Z, dimenssions of your blank stock.
- Use the variables of those ecuations to define "custom properties" which you can add to BOM tables on your drawings.
Several months ago I post several examples on how to do this, do a seach for "blank dimensions" and you will find them.