Technique for Building with Aluminum Extrusion 1

[SoledWorker]

I'm interested in learning how people are handling the use of extruded aluminum profile in SWX assemblies. (Used for guard framing, machine bases, etc.)

Ideally, I'd like to build by extruding the profile mat'l from a face of the frame up to another surface. This could be handled by inserting a new part, but how to track the length so that it can be included in the BOM?

Configurations would get very messy, because ANY length may be needed, this would lead to a huge number of configurations.

Individual part files could be used, but if the part file name (1515_x_31_inch.sldprt) contains the length, it won't update if I change the frame and the extruded length changes. Plus, to name the part, I'd need to first measure the distance...

 

[DetroitPickles]

Are you indicating that the extruded length is not the same as the length of the part?

If it is, you can put the extruded length into a Custom Property that is used in the BOM.

Mr. Pickles

 

[RawheadRex]

"...you can put the extruded length into a Custom Property that is used in the BOM."

This is what I recommend as well although depending upon what's important to you, you may find it necessary to customize the BOM template.

I have a seperate BOM format that I use when dealing with weldments and the like which reads custom properties containing the length information and displays them on a drawing. Another thing that you could do is have standard generic part models designating different extrusion profiles.

Following along the same lines of thinking you mentioned above, you would just make as many copies of the generic models as needed for different lengths that you require BUT don't included the lengths in the part name (as you already alluded to, this is a major pain in the a**). Of course each individual part needs to have a unique name so you have to deal with that. In the way of suggestion, I get around this by assigning a part number that is used only for purposes of managing the model in SolidWorks to each individual model under this scenario. Depending on your part numbering scheme this may work out well for some but not others.

Hope this helps.

Chris Gervais
Mechanical Designer
American Superconductor

 

[Stoker]

I will assume that the aluminum profiles can be used on many different assemblies and that you want to define the length of the base-extrude as "up to surface" or "up to vertex" so that the length of the extrusion updates as the rest of the assembly is changed. If you think about it, the only way to accomplish this within a single part file is to create mulitple independent features (configurations). There is no other choice within one part file. You will pay a big price for this. Usually, most people treat extrusion profiles in a similar fashion to other off-the-shelf items. They go in the part library and get pulled into assemblies from there. Creating a single part with references to multiple assemblies and then putting it in the library is a VERY bad idea, if this is what you are doing.

There is a way to have your extrusion profile in the library, have the "up to surface" definition for the base-extrude and get the length in the BOM. Create a profile sketch and extrude it 0.001" and put this profile "part" into the library. When you need an assembly with this extrusion, create a derived part (insert->base part) and position it on the first face. Then edit the part in the context of the assembly, convert entities on the profile face and extrude up to the desired surface. Add a reference dimension on the length and put this in the BOM.

 

[TateJ]

I have a part for you to check out.
There's some "code" in the $PRP@DESCRIPTION property that reads the distance from an annotation... blah blah blah.
I think it'll do what you want.
I wish I could take credit for this - I stole it from a buddy at work.

Never-the-less, post your e-mail and I'll send it to you.

​

tatej@usfilter.com​

aka: Little Debbie's Boy-Toy​

 

[skiking]

I am the design engineer of a shower door manufacturer. We use multiple shapes of aluminum extrusions and plastic parts, glass and vinyl extrusions to make our shower doors. I have made assemblies of almost all our line of shower doors. I use full size units to check for fit and function and sample sizes units for publications such as instruction sheets and details views so that the customer can see the shape. I have accomplished this by using design tables.

 

[enginerd1959]

We face a similar situation. We do custom machine design, and the lengths of our extruded frame parts can be anywhere from about 100mm to 5600mm. If we round off to the nearest millimeter that's 5500 part possibilities - most of which we'll never use.

Our VAR has suggested that we purchase and modify the SWX piping module to handle designing with extruded parts. Instead of round pipes, use the special rectangular profile. This would seem a good approach, as the piping module tracks the length of "pipes" and reports them on the BOM. Has anyone tried this?

 

[EdDanzer]

The fastest way to use bar shapes and end up with shop drawing of components is to create a reference part with reference geometry, save it as a reference part of that shape. Create a drawing page with the reference part in it with general dimensions and BOM then save it as a reference drawing of that shape. When you need the bar shape, open the reference part and drawing. Do a file save as on the drawing with the part number to be used for manufacturing, save the reference part with the same part number. Now you are ready to adjust the solid model as required to fit. The drawing page will up date and is ready for additional dimensioning. If you use file properties to define information about the material etc., it will update also. Be sure to use the same base model and drawing for all similar shapes, and if possible use mating geometry when assembling, that way if you need to change bar size the mates won't be lost. This method works great for assembly families where only some parts change size.

 

[macPT]

Well, again it seems that there's a lot of different ideas and experiences, and I am shure that we can't name one that serves all of us. The solution depends a lot on your organization, on your product type and on your design intent. What is good for one person can be bad for another. But I will explain how I deal with yhis problem. First, I create, on a standard components folder, a part having the correct sketh of the profile and a generic length (whitch is a configuration). If the component as some extra machining (that is, if it's not only cuted raw material and as extra work like drilling) than we copy the sketch from the standard part and design a new part with it's own code. If the component it's only cuted and used in an assembly, we create a configuration of the standard part with the needed lenght, the code is the raw material's code (the standard part's code) and the length is in an information column in the BOM. Until now, we are doing fine with this procedure.

Regards

 

[SnowCrash]

The profiles of the extrusions you use are supplied by the manufacturers who seem to have copied them from some common profile. They are available from the vendors on CDROM.
My experience with them has been poor. The profile sketches are too complex and are very unfinished and do not close up. Better to start from scratch.
I create new configurations for each new size I use. If the size I want exists I just use it from the config tab. The config name is the decimal length. The profile is the text definition in the BOM.

Crashj 'keeps a low profile' Johnson

 

[Standing]

TateJ
I would like to check out the part that has “code” in the $PRP@DESCRIPTION property that reads the distance from an annotation. I have been trying to find out someway of reading values in an annotation.
Thanks for your help.
brad_johnson@dstoutput.com
Bradley

 

[dhinners]

You can get the length of a part into the description as follows:

Start your custom properties editing in the part as usual with File, Properties. Then switch to the 'configuration specific' tab and select the 'description' property (or whichever you use in your BOM description field. In order to get values from annotations, type in the text portion, then double click your part (with the property dialogue still open) and click the text of the annotion you want. So, for example, you can type:
'ALUM. EXTRUSION, '
Then select from your profile sketch an overall dim showing the extrusion size. Next you type:
'MM SQ. X '
Now you can select the extrude length dim. Finally, finish it off with your desired text at the end, such as:
' MM LG.'
Remember to click Add or modify!
When you select the dims, Solidworks automatically puts code in the property which reads the value. You will see something like '"D1@Sketch1@@Default@Part1.Sldprt"'

When the BOM reads the property from the example above, it will show:
'ALUM. EXTRUSION, 40MM SQ. X 232 MM LG.

 

[Mindnumb]

Have you tried the piping add in?

It has the exact feture you describe. all pipes are generated from a set of profile configurations, and then for each assembly i generates a set of lenght configurations for each size. Pipe lengths ar then listed in the Bom.

I tried to apply it for square ducts, but I had problems with the orientation of the elbows and That the straight ducts tend to spin 45 degrees about its lengt axis, so I gave up. Anyone else tried Alternative Profiles in the Piping module?

Anyways, te most decent method seem to be te same as the piping module does, just do it manually.

Create a part with the different profile configurations (sizes), it might be smart to maked different parts for profiles that does not have the same shape...

then use save as, and give the profile a unike name for every assembly its used in, and make confiurations for every different lenght in that assembly. DO NOT link the configuration name to the lengt because that might change, use the method described in posts above on how to read the lenght to BOM.

Most fun would be to incorporate all kinds of profiles to piping, but... Have to try that later some time.


good luck.

 

[SBaugh]

Reading Values in in using an Annotation is easy when you go to the properties and click on the link button in the lower right corner. You can link it to information stored in either your DT or in the Custom Properties of the part or Assembly.

HTH, Scott Baugh, CSWP
3DVision Technologies
credence69@REMOVEhotmail.com

http://www.3dvisiontech.com

http://www.3dmca.com

*When in doubt always check the help*

 

[SeanF]

For what it is worth... This may not be the best way but it is the way that I have decided to handle such matters as I have a VERY similer extrusion "problem". So here goes.

I use derived component parts. I know, this is not great because SldWks will not let you make such things from stand alone parts. So I have to keep an extra asm floating around. However, this makes it so that I can have a file that drives the shape of many, and at the same time have the many be isolated from each other as well as NOT update the extrusion profile. Most of our extrusions get machined in some way. Of course they don't get the same cutting as that would be too simple. So doing this way solved some problems for me. Now the shape of the base extrusion can be dealt with in one place at the same time updating all related parts as needed. This keeps file names in line for me as well. This for us is important as ERP/MRP tracks the extrusion as a seprate part number that is more or less "attached" to the finished part, that of course will have a different part number from the base extrusion. So, for me doing things this way has worked well for me.

Regards,

Sean F

 

[Foundation2]

If your guarding or machine bases are quite similar, you can create master templates (assemblies).
Each of these would have a "Master sketch" which has your main parameters; width, lentgh, height, etc..
This sketch could drive all dimensional properties of your components via equations and/or design tables. You can create quite complex and sophisticated templates. Dimensional values can then be exported to your BOM's.
Later, this could also be used as a quote/costing tool.
How complex and sophisticated they get, it will depends how much time you are willing to invest to create them.

Good luck
Marek K
Marek Karczmarczyk
MD-PM Inc.

http://www.sentex.net/~marekk