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I am a beginer and I want to automatize things and don't know how.

Question asked by Eugen Lupascu on Sep 1, 2016
Latest reply on Sep 6, 2016 by Christian Chu

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I have this Panel which I think isn't made well.

All the profiles you see are sheet metal. I have to do a configuration of it. How can I connect all the parts toghether that when I modify the overall Lenght, Height and maybe Width all the distances and the components inside to be automaticaly updated.

I have to mention that the model is highly parametrised and all the mates are made between planes and axes, and for a modification I have to spend a half of hour.

The exterior profiles, those which compose the frame are a single part with multiple configurations, and the interior profiles are one part with multiple configuration.

I tried with an ecuation but that changes all my configuration and I don't want that.

Will I have to have a single assembly without configuration formed by parts with one configuration connected through ecuations or I can have Assembly with multiple configuration formed from Partswith multiple configuration and all the dimesions to be connected throught ecuations between dimensions from parts and assembly?

I made the parts sheet metal because I cut them in laser.

If you dind't understand please tell me! Thank you!

John Stoltzfus Sep 2, 2016 8:16 AM

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A complicated pc a simple pc, I start "All" my projects that way, it was just quicker for me to show a simple assembly. It definitely takes more thought in laying it out, but the end result is pretty awesome when you have to make changes or delete any item in the feature tree, suppose you change your design mid stream, there will be some components that are ok, but if you're not careful in your design intent, your entire assembly can blow up by deleting one simple part or changing it from rectangle to round etc..

You can simply do what you want, I just know what works consistently for me...

Save a copy of the simple assembly in a different directory, then go and delete any item, change the sizes, check for interference's, delete the main assembly and start a new assembly and insert 9001 9002 9003 assemblies and see what happens, no mates to clog up the top assembly and you can work in zones, no need to work in the top assembly anytime.

Just my penny thoughts.....

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J. Mather Sep 1, 2016 7:46 AM
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I recommend that you first attach your assembly here to have experienced users take a look.

Have you gone through the Weldments tutorials?
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Gianluca Mattaroccia Sep 1, 2016 7:51 AM
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Eugen, in my humble opinion you can solve this issue very easily by re-drawing your frame with Weldments.
That allows you to start from a 3D sketch that you can modify with ease and create relations with formulas if you desire. You can create the same frame with different profiles as well.
I am attaching a sample of something I was working on the other day. No need to spend time in creating parts and mating them the hard way. The beauty of this method is that you also deal with a single part file instead of 1 assy and multiple parts. As far as drawing concerns you will be able to create a cut list showing all your members, cross section name and length and more if you like.
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- Gianluca Mattaroccia @ Gianluca Mattaroccia on Sep 1, 2016 7:50 AM
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  Forgot to attach all the pictures...
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  - 5.PNG33.4 KB
  - 4.PNG16.9 KB
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  - Eugen Lupascu @ Gianluca Mattaroccia on Sep 1, 2016 8:44 AM
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    What are you showing me is a simple frame made in weldments. I don't know if you observe but the side, up and down profiles have holls in it for bolts. The interior vertical profiles are mirrored one to each other as same as the horizontal profiles ( the 3 ones from above are mirored with the 4 ones from bellow, so I think a liniar pattern cannot work in this case.
    Thank you!
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    - Paul Risley @ Eugen Lupascu on Sep 1, 2016 9:51 AM
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      In a weldment you can mirrror parts, you can mirror bodies(tubes with holes in them). I agree with Gianluca the screenshot you provided screams weldment & configurations of that weldment to achieve your end desire. You would then get 1 part that you can detail out anyway you like and control only that part vs. having individual tube parts that have mates and hole patterns and configurations. The weldment would give you one clean part that is easy to manage both now & in future revisions if necessary.
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      - Paul Risley @ Paul Risley on Sep 1, 2016 10:02 AM
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        I forgot to insert this on my last response. This is almost completely done in weldments. It is an automated Robotic machining center the blue frame is all 1 pc. Yet when built it breaks down into 5 separate sub weldments. The carriage trolley is 1 pc as well broken down into several sub weldments. I designed this around a concept for the nesting of the parts we had to machine. 1 3d sketch drives everything, so I can change the sketch in the main assembly and it updates all of the weldment parts. So what I am saying is what you are showing and what you want to do in your part is totally do-able. You just have to figure out what your final product needs and apply it in a fashion that makes sense to you. If it was me I would make it weldments and add the configurations or design tables as needed to make it work.
        Good luck.
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    - Gianluca Mattaroccia @ Eugen Lupascu on Sep 1, 2016 9:57 AM
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      Eugen, I have only attached a sample of how it is done.
      If you need to add holes you can do that in weldments as well. You can flip profiles, change their orientation, location, you name it. It is the most powerful tool for this type of work. Just my two cents
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    - Chris Mackedanz @ Eugen Lupascu on Sep 2, 2016 8:10 AM
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      If you look at the configurations in a weldment there is usually 2 configurations, an <As Machined> and an <As Welded>. The welded on will be a derived configuration of the machined.
      
      When you add cuts into a weldment, if that cut only goes through one member of a group of identical members SolidWorks does actually realize that this one member is different than the rest and if you look in your cut list you will be able to find just that one single member listed.
      
      Unfortunately you can not have those holes come in automatically as part of the weldment, like if you want to use some square structural tubing which has holes on all 4 sides every so many inches apart, those holes will not come in. At least not that I'm aware of.
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      - Paul Risley @ Chris Mackedanz on Sep 2, 2016 8:56 AM
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        Chris,
        
        That is the default setting which you can turn off. It works for simple weldments, however if you add a configuration to your weldment it then has <as machined>, <as welded>, configurations as well. You can turn that off under options>document properties>weldments> Uncheck the box (Create derived configurations).
        Like I said on simple weldments not a big deal but if you are working on larger projects with lots of weldments it bogs down solidworks pretty bad.
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        Chris Mackedanz @ Paul Risley on Sep 6, 2016 8:32 AM
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        That's true, I was just using them as an example that SolidWorks does handle any solid body with cuts as separate bodies. (Unless they are exactly identical)
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John Stoltzfus Sep 2, 2016 6:58 AM
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Eugen Lupascu As with anything else there are multiple ways to start any project and through the years many of us tried all kinds of different methods, therefore you may get a few suggestions. The other important part in the design process is the "Company Policies" & "Industry" which can take different approaches.

I will share a proven design intent - "what worked best for me" For every project I create a dummy part which I call a Skeleton Sketch part and all my geometries, planes, axis, surfaces or anything else that I need for the entire assembly. This part is then inserted in every Assembly, main and sub.

Attached is a draft of my workflow and if you have any questions let me know..

Edited - I attached a sample file - Unzip it and try it
Attachments
- Cabinet-Sketch.zip3.4 MB
- Solidworks Work Flow-A.pdf1.0 MB
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- Eugen Lupascu @ John Stoltzfus on Sep 2, 2016 7:42 AM
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  I see what you did. Is very amazing but I can see you work in the furniture industry. The machine which contain that particular panel frame is a smoking chamber, so I think is more difficult to built it in your way.
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  - John Stoltzfus @ Eugen Lupascu on Sep 2, 2016 8:16 AM
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    A complicated pc a simple pc, I start "All" my projects that way, it was just quicker for me to show a simple assembly. It definitely takes more thought in laying it out, but the end result is pretty awesome when you have to make changes or delete any item in the feature tree, suppose you change your design mid stream, there will be some components that are ok, but if you're not careful in your design intent, your entire assembly can blow up by deleting one simple part or changing it from rectangle to round etc..
    
    You can simply do what you want, I just know what works consistently for me...
    
    Save a copy of the simple assembly in a different directory, then go and delete any item, change the sizes, check for interference's, delete the main assembly and start a new assembly and insert 9001 9002 9003 assemblies and see what happens, no mates to clog up the top assembly and you can work in zones, no need to work in the top assembly anytime.
    
    Just my penny thoughts.....
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  - Peter De Vlieger @ Eugen Lupascu on Sep 6, 2016 10:57 AM
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    Eugen,
    
    For what it is worth, we use a method very similiar to John's.
    By which I mean, using a skeleton sketch, using the origin of the top ASM as the absolute base point for each top level sub-ASM, working with planes to drive location, working in zones that are independent of each other, etc...
    
    We use a simplified version of that method for small skids with a scubber for instance.
    We use the full version for complete Biogas plants with a few kilometers of piping. So if we can design a complete factory with it (including piping and supporting structures for the piping) then a smoking chamber can't be too difficult for using that method.
    
    Having said that, if you want a truly easy way then you really should check out weldments.
    I agree with Gianluca Mattaroccia and Paul Risley , what you've shown us seems to just beg for a weldments solution.
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  - John Stoltzfus @ Eugen Lupascu on Sep 6, 2016 11:09 AM
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    The only thing missing with our design intent is a macro button with a voice command "Design Me A New Car", we go for coffee, we get back and the latest and greatest car is designed and ready for production, (rant)
    
    There is no way you can look at something in 5 minutes and say that's not for me it's too simple, without knowing what's in it, lol - It is good to gather a lot of information, however I still feel that you need to find out on your own which approach is best and there is no way to know till you pick one and go, till then have an awesome day
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Christian Chu Sep 6, 2016 11:15 AM
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I would use a master sketch and adapt all parts to the sketch - so basically, you use the master sketch to control parts size and the assembly
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