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Family of Custom Profiles

Question asked by Rob Edwards on Aug 30, 2017
Latest reply on Sep 1, 2017 by Dave Bear

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Morning All

Just starting a new project and thought I'd create some Custom Weldment Profiles.

Here are a couple of them - there are lots more!

As you can see they are similar but too different for a single sketch/ configured. During development it would be nice if I could link them together.

Is there a nice way to link them so that if I change one the other changes?

My initial thoughts in rough order of preference...

It would be really nice if I could use a single configured profile, suppress one sketch or the other?? (doubt possible)
Define multiple custom profile sketches in a single part file linked to a master sketch?? (doubt possible)
Create multiple part files that each create a custom profile in the context of an assembly containing a master sketch (seems feasible)
Do something with a block
Create just one profile and mirror it in the part (other variations would need additional features)
add relations to the profile sketches in the part that link them together (probably what I'll do)
abandon the idea of using custom weldments and make cuts in the part (just use a square weldment profile)
create a weldment profile that is the negative space and use a combine/subtract feature
manually edit separate profile files

I've not yet tried any of this - hoping someone can chime in with a better idea before I end up in a rabbit hole.

Thanks in Advance

Dan Pihlaja Aug 30, 2017 1:32 PM

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Here is another option of using a single text file to control all of your global variables and equations for multiple parts:

Sharing Variables and Equations Between Models

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John Stoltzfus Aug 30, 2017 8:09 AM
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I have all my mouldings as Blocks, very easy to use.. If you need to modify one - easy again just explode the block, add relations accordingly..
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Rob Edwards @ John Stoltzfus on Aug 30, 2017 9:19 AM
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Cheers John
Yes Blocks are great for all our tooling, but I really wanted to use a custom weldment profile for this panelling project.
I was thinking of dropping a block into each of my .sldlfp files ( a bit like your skeleton method) and then referencing it in the sketch used for creating the profile. I haven't tried it yet but I guess external references may not be allowed at all.
Maybe a linked design table would work, I know they work with custom profiles.
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John Stoltzfus @ Rob Edwards on Aug 30, 2017 9:24 AM
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You need a sketch for your weldments, not?? - so just drop your block in there and that way if you have another project or need to add a small block that you just need to extrude a little, then you have the sketch setup as a block, that would give you versatility to go either way..
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Rob Edwards @ John Stoltzfus on Aug 30, 2017 9:52 AM
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Thanks again.. I'm going to give it a try. These profiles are constructed from multiple machining operations with various cutters (blocks). The more I think about it, maybe I need to go down the part/assembly route instead of a weldment. (although it would be great for woodworking if we could do this)
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John Stoltzfus @ Rob Edwards on Aug 30, 2017 10:01 AM
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I wouldn't give up on weldments, if that's what you wanted to use. There is a sketch inside the weldments, isn't there? All I'm saying is set up your profile blocks first and then when you create your weldment profiles, insert the block in the sketch and then save it out as a weldment part, or you could start your sketch for the weldment and then save out a block from there.. Either way, you sketch it, then save the sketch as a block as well, that way you can have the ends of both worlds...
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Dan Pihlaja @ Rob Edwards on Aug 30, 2017 9:57 AM
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If you are going to go down the part/assembly route,

Then create a single part with all the profiles in it. Make one master sketch inside that part and then link all the other sketches inside that part to the master sketch.

Then you have 2 options:

1) Save that part as a template, and just use it for all your components (using only the sketch that you need).

or

2) add that part to all your assemblies (as the first part), then make your parts with in context relations back to the first part (using "insert" --> "derived sketch") to drive all the profiles of your parts.
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Rob Edwards @ Rob Edwards on Aug 30, 2017 1:07 PM
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Thanks for all the input guys, here's where I am so far

I've got a simple example going with a linked design table. I've not used the files as profiles yet, still just parts.

I added both sketches to a part and then added a DT. I saved the DT, deleted it and re-added with link to file. I allow model edits to update the table.
I then saved a copy of the part, but the beauty is there's still only one DT.

Now when editing one part the changes come through to the other.

I'm not quite sure what to do with this dialog, I'm guessing this is where it could go wrong.

Anyway I'll try turning it into profiles now

EDIT:
Doesn't work, causes SW to crash
Attachments
- Panel Profile Sample2.SLDPRT.zip52.2 KB
- Panel Profile Sample.xlsx9.2 KB
- Panel Profile Sample.SLDPRT.zip52.0 KB
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Dan Pihlaja @ Rob Edwards on Aug 30, 2017 1:41 PM
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Family of Custom Profiles Edit: (can't believe I accidentally linked this very thread to this very thread.....I almost created an infinite loop!!)

Using one Design Table (Excel file) for Multiple Parts

Try this:

Create 1 excel document that is your "master" and not directly linked to anything in Solidworks
Then Create each of your profiles in separate parts inside Solidworks. Create an external design table for each part in excel.
Then link the design tables to the Master excel file.
Then modifying the Master excel file will update the other external design tables.

Edit: Disclaimer: I haven't actually tried this. I could see an issue where the excel files have to be opened to update. But maybe that will happen when you open the part.
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Dan Pihlaja @ Rob Edwards on Aug 30, 2017 1:32 PM
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Here is another option of using a single text file to control all of your global variables and equations for multiple parts:
Sharing Variables and Equations Between Models
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Rob Edwards @ Dan Pihlaja on Aug 30, 2017 1:51 PM
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Hey Dan

I like your thinking in the first suggestion, but I gave up on that. As for the second, that's what I just did and it works a treat!
I'm still interested in looking at other methods, so if you don't mind I won't mark your answer as correct, but it does work..
YES!!

EDIT:
This does seem pretty cool to me. It use's global variables and my text file is linked to the weldment profiles AND the weldment part.
It isn't strictly necessary to link them like this and possibly a bit dangerous. The cool bit is that equations defined in the sldlfp pass through to the part. All my equations just used the same named global variable, easy peasy really. I'll upload the part when I'm finished
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Dan Pihlaja @ Rob Edwards on Aug 30, 2017 1:44 PM
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Rob Edwards wrote:

Hey Dan

I like your thinking in the first suggestion, but I gave up on that. As for the second, that's what I just did and it works a treat!
...
I'm still interested in looking at other methods, so if you don't mind I won't mark your answer as correct, but it does work..
YES!!
I think that you can even import the text file into a blank part and then save it as a template. That way you won't have to do it multiple times.

Awesome!
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Rob Edwards @ Dan Pihlaja on Aug 30, 2017 1:53 PM
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Awesome indeed
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Dave Bear Aug 30, 2017 8:12 AM
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Hi Rob,
I thought you'd fallen off the planet.......... lol

I'm guessing these are regular mouldings that you use? I wonder if John Stoltzfus has ever ventured through anything like this?
As a side interest (I'm a qualified Wood Machinist/Cabinet Maker by trade), do you ever make your own custom cutters in-house?

I'm really interested in seeing the results of this thread!

Dave.

**** EDIT **** Haha, John piped up seconds before me!!!!!!
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Rob Edwards @ Dave Bear on Aug 30, 2017 9:41 AM
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Thanks Dave
Yep I've been busy, doing some 'real' work. I had about a month in the workshop and on-site. It was a bit strange picking up my tools again... and now it's a bit strange sitting at the computer.
We don't make our tooling in house (except for scratch stocks from old hack saw blades). It's so cheap these days,,, just draw it up in SW, e-mail the dxf and bingo, about a week later there it is by magic!!
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Dave Bear @ Rob Edwards on Aug 30, 2017 9:43 AM
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Jack of all trades...............

Dave.
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Rob Edwards @ Dave Bear on Aug 30, 2017 10:01 AM
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.....Master of none!

Love that expression. Our company's called Jack Badger - inspired by the wood plane. Do you call them Jack Planes in down under?
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Dave Bear @ Rob Edwards on Aug 30, 2017 11:37 PM
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No Rob,
Down here the technical name is "Surface Plane(r)" but everyone just calls them a "Buzzer"
And as for "Spindle Moulders", well we just call them "Shapers"
Pretty much everthing in Oz has a nickname!!!!!!!!

Dave.
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Rob Edwards @ Dave Bear on Aug 31, 2017 1:57 PM
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On the "buzzer" - I like that. We're boring, just call it a planer, or surfacer. What I meant by Jack plane was a bit more old school
Jack Plane, shorter than a tri plane, longer that a smoothing plane. Can do both jobs but not as well.
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Dave Bear @ Rob Edwards on Sep 1, 2017 7:13 AM
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Oh! Sorry, That's just a "plane" (hand plane).
No exciting name for that one! lol.

Dave.
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Todd Blacksher Aug 30, 2017 9:53 AM
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Rob,
I've been meaning to create a post to show a technique, but I haven't gotten around to it yet. (although I will be showing it for slugme)

Here is something to consider (Huge apologies that I don't have a sample with me to upload):
I used to use a lot of standard aircraft extrusion, and we would set up a template with the sketch (as you have shown above), along with all of the information for the part, and a design table with all of the possible configurations.
Since we were mostly top-down modeling, this worked great - If you needed two brackets for a shelf, just insert a new part, select the template for the extrusion that is needed, click on the sketch and extrude it to length.
We would have a template file for each "family" of extrusion (L-bracket with equal length legs, L-bracket with unequal length legs, H-Channel, U-Channel, J-Channel, and so on) - Each of these templates would have configurations for the different sizes.
It worked very well for our specific application, however since we didn't use them for weldment type structures, we never pursued that avenue.
I'll try to upload a sample later . . .
todd
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Glenn Schroeder Aug 30, 2017 10:14 AM
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Rob,

I love using weldments, but when using the Structural Member function it just copies the .sldlfp sketch and doesn't maintain a link to it, so if you want profile sketches linked I don't see how it can work.
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Rob Edwards @ Glenn Schroeder on Aug 30, 2017 10:58 AM
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Thanks Glenn

Yes I would have to manually update each structural member, which isn't ideal. This is more for use in development, where I want to tinker with dimensions without having to manually edit *all* of my profiles. I've noticed if you make sure that you never reorient the profile (eg mirror or use a different point) it updates pretty quick.
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Oliver Washington Aug 30, 2017 10:36 AM
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Hi Rob,

I created a series of guides on custom weldment profiles a while ago. These should instruct you on how to create particular configurations and save them out as custom Weldment Profiles. There's also details about the save structure too. These files are attached.

Olly
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Rob Edwards @ Oliver Washington on Aug 30, 2017 10:58 AM
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Thanks for sharing Oliver
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