Two Questions Dealing with Top-Down Assemblies

[DBCox]

Hello everyone,

I am relatively new to SW and a complete newby when it comes to top-down assemblies. I have been reading up on them online and have come to the conclusion that my best bet is to create a layout drawing of my assembly (I can represent it in a single layout view in 2d. I can then create each part of the assembly from that single layout....Theoretically.

I am running into two problems when I try this and hopefully you can help.

1. I cannot seem to create a part from the layout, even when changing it to a block. However, I was able to "roughy" the sketch in on a new part and then constrain all of the lines to the layout as co-linear. That seems to work, but it is cumbersome when I have to sketch it twice (once for the layout and once for the part) and then constrain it. What is the proper and efficient way to create a part from the layout?

2. I drew my first part of the assembly and "traced" it as described in #1 above and create a part that seems to do what I want it to (it updates when the layout updates). However, now I need to sketch the other part in the layout and am having trouble. This entire assembly is round and modeled using revolves. When I try to sketch the additional part into my layout, SW will not allow me to dimension a diameter off of my centerline. It did on the first part. Is this becuase I am adding to the layout?

I am using SW 2008 if it matters.

 

[ShaggyPE]

Don't know if you have access to the SolidWorks forums, but here are a few links.

https://forum.solidworks.com/message/118659

https://forum.solidworks.com/thread/14544

Check out the posts specifically by Mauricio Martinez-Saez

-Dustin
Professional Engineer
Certified SolidWorks Professional
Certified COSMOSWorks Designer Specialist
Certified SolidWorks Advanced Sheet Metal Specialist

 

[drawoh]

blakrapter,

I do not quite understand what you are doing. I have embedded sketches at the assembly level, and used these to control the parts attached to the assembly. This is not different than using features of one part to control features of another part.

When you create new parts for top-down design, attach your key features to your origin, and use these to mate the part to your assembly. You can use driven features as assembly mates, but the updates will be unpredictable, and you will have a lot of weird failures.

JHG

 

[fcsuper]

It sounds like you are mixing methods and coming up with the resulting results. What is your goal, and let's work for a solution from there.

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

 

[DBCox]

Thanks for the quick reply guys!

Shaggy, thanks for the links to the SW site. I read some of Mauricio's posts that got me started, and those helped some. I will say though that they were over my head for the most part. Unfortunately, I do not have access to the SW forum to post.

Drawoh's sketch method helped quite a bit. It seemed to work better than the layout sketch method I was using. I am still running into a couple of problems though.

So, I think Matt has the best idea about letting me explain what I am trying to do so you all know what I am up against. I am trying to create a generic assembly file that I can fully define with a series of equations and variables. These are the key characteristics of the assembly. Once the assembly has updated itself, I need each part file saved individually for CNC purposes and I need to create drawing files for all of them. The drawing files can be linked to individual parts within the assembly, or the individual part files, either is fine. Since the file is generic (essentially a template), I need SW to automatically rename all part and drawing files and components within the assembly when I save the assembly as a new file. Specifically, I am doing the following:

I am modeling an assembly of a hydraulic cylinder that has about 5 basic components. I am modeling it to be generic and then defined by equations. The entire assembly can easily be represented in a 2d section view, but of course this does not give me mass properties, or the ability to easily add specific features that are not represented in the section view. Because of this, I would like to revolve each part to make it 3d. I have successfully created sketches at the assembly level and driven them with equations.

My problem is getting them into individual part files. I took Drawoh’s suggestion of sketches rather than layouts at the assembly level and that seems to work better. Similar to the layout method I described in my initial post, I "traced" the sketch associated with the part I was creating. For instance, the end cap. I have a sketch called end cap at the assembly level and then created a component called "End Cap." To create the revolved part, I created a sketch within "End Cap" and traced the sketch at the assembly level. This seems to work great, but I do have 2 problems:

1. I cannot figure out how to automatically name the parts for each assembly. For instance, the assembly may be called Generic-1234. It would be great if I opened my generic assembly file, "save as" to Job-1234 and then each component associated with it would update its name and save as a separate part file (not imbedded in the assembly). For instance, Generic-1234-End Cap would change to Job-1234-End Cap when I used the save as command.

2. When defining the sketches in the assembly level (the ones I "traced" to create each component sketch/revolve), I defined tolerances to some dimensions. These are not being transferred to the parts. When I create a drawing of them, the tolerances and not available. I am sure this is due to the tracing method, but I do not know how to get around it.

Sorry for the long post, but I hope I was able to clarify what I am trying to do. Any help will be greatly appreciated!

 

[CorBlimeyLimey]

blakrapter ... Did you notice that Mauricio uses the older Top Level sketch-in-a-part method rather than the Layout function?

The two methods are similar and both have their uses, but the Layout function has limitations and can create some peculiarities in certain situations.

 

[AnnaWood]

blakrapter,

Sign up for an account on the SolidWorks forum and you will be able to post questions there as well.

Cheers,

Anna Wood
Anna Built Workstation, Core i7 EE965, FirePro V8700, 12 gigs of RAM, OCZ Vertex 120 Gig SSD
SW2009 SP3.0, Windows 7 RC1

http://www.solidmuse.com

http://www.phxswug.com

 

[rollupswx]

Sign up for an account on the SolidWorks forum and you will be able to post questions there as well.[/qoute]

Been there, done that. Twice. After submitting critical comments about Hole Wizard, log-in no longer worked.

 

[DBCox]

Thanks for the info guys. I am unable to sign up for the SW forum because I do not have a service agreement. I wish I did, but do not have access to it unfortunately.

Any ideas from the folks here?

Thanks!

 

[AnnaWood]

Sigh....... You do not need a service agreement to sign-up on the SW forums.

Cheers,

Anna Wood
Anna Built Workstation, Core i7 EE965, FirePro V8700, 12 gigs of RAM, OCZ Vertex 120 Gig SSD
SW2009 SP3.0, Windows 7 RC1

http://www.solidmuse.com

http://www.phxswug.com

 

[ShaggyPE]

Regarding your question #1. That isn't going to be as automatic as you wish, but there are two methods that I see working reasonably well.
1. SaveAs and click on the references button in the save dialog prior to hitting ok. This will allow you to manually rename every part in the assy to a new unique name.

2. Pack-N-Go. I have not used pack-n-go because alas I am stuck doing my work in 2006. My understanding is that pack-n-go will gather up all of the files related to an assy (drawings of piece parts as well) and save them to a new location. You will have the ability to rename them at this time as well. Possibly someone else can clarify this direction, or do a help search on it.

-Dustin
Professional Engineer
Certified SolidWorks Professional
Certified COSMOSWorks Designer Specialist
Certified SolidWorks Advanced Sheet Metal Specialist

 

[DBCox]

Shaggy,

Thanks for the info. In all honesty, I guess I cannot complain about having to re-name a few files if it saves me all of the other time. I haven't had a chance to try it, but I think it has a find/replace function too, which could make it pretty quick.

Anna, how did you get access to the forum without an active subscription? I have an account for the SW Community, but there is a lock next to "Forums" as well as other sections. The note at the top next to the lock icon says "Active subscription service contract required for full access"

Any help on using those assembly level sketches in the individual components will be greatly appreciated!

Thanks!

 

[rgrayclamps]

Hi, blakrapter:

Top level layout sketch is the way to go. You need to create sketches on your top level assembly. Then, you create sketches in individual parts via in-context relations according to your needs.

When you finish your assembly and its components, you can rename or save them (all of them, I mean, the assembly model, its drawing, all the parts, and their drawings) automatically or selectively, or manually one by one.

Good Luck!

Alex

 

[DBCox]

Alex,

Thanks for the quick reply. Your described method seems the most logical to me. I have actually tried it but had problems with dimensioning with tolerances (see my second post above).

This may be a drawing problem rather than modeling problem. Because, I was able to bring the entire assembly in with only 1 component visible and dimension it with the "Model Items" command, but this did not seem to work when I brough each individual part file in. Also, weired stuff seemed to happen when I did this. For instance, large greyed out center marks and axis lines came in.

Should I be bringing in the assembly and hiding all components except the one(s) I need to dimension, or should I bring in each part individually?

Thanks!

 

[CorBlimeyLimey]

If you use the TL sketch-and-convert method, the Insert > Model Items function will not bring in the dimensions because they are attached to the TL sketch not the converted part sketches.

Dimensions will have to be added manually if individual parts are detailed on drawings, but that is a far better than adding in the whole assy and hiding all but one part for each part detail.

 

[AnnaWood]

blakrapter,

You need to ignore what the Customer Portal tells you it is screwed up.

http://www.solidworks.com/sw/support/FAQ-CustomerCenter.htm

Use the link below and login where it asks you to log in if you have a Customer Portal account already.

https://forum.solidworks.com/index.jspa

Cheers,

Anna Wood
Anna Built Workstation, Core i7 EE965, FirePro V8700, 12 gigs of RAM, OCZ Vertex 120 Gig SSD
SW2009 SP3.0, Windows 7 RC1

http://www.solidmuse.com

http://www.phxswug.com

 

[rgrayclamps]

Hi, blakrapter:

Why would you want to bring an assembly into a drawing view and hide all parts except one? It seems that does not make any sense. There is nothing to hide. If you want to detail a part, you make a drawing for the part. If you want to detail the assembly, you make an assembly drawing. If you really want to hide some parts, you need to make those invisible from the view but not from the assembly model.

Layout sketches in assembly are for your design intents. Tolerances should be handled in parts' models. You can then import them into their drawings, or handle them through drawing documents.

Good Luck again!

Alex