Idea for an enhancement request? 3

[MattP]

I often run into problems when making major revisions to assemblies, finding it difficult to understand quickly which mates are doing what. Sometimes it seems easier just to delete ALL of the mates and start from scratch. I am aware of some/most of the tricks to see which mates pertain to which part (ie: View Mates, View Dependencies, renaming mates, etc.) but they seem to only help marginally. What if there was a tool that when you tried to drag a part in a particular direction, SW would point out to you which mates were preventing the movement instead of just telling you that the "...component is fully defined..." What do you think? Would something like this work?

 

[MadMango]

That sounds like a nice feature. It would be nice if you could also add Folders to the Mate tree to better organize Mates. You could also force your users to rename the Mates so they are easier to undertand, making them user friendly.

Ray Reynolds
"There is no reason anyone would want a computer in their home."
Ken Olson, president, chairman and founder of Digital Equipment Corp., 1977
Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[mncad]

MadMango,

I believe you can already put the mates into folders and rename them. At least you can in SW2004. Not sure that you can force the renaming though.

mncad

 

[Timelord]

Folders are available to organize mates in 2004 SP 3.0 and you have always been allowed to rename them. Also, the "mates in assemble" folder at the top of the individual parts feature list makes it easy to understand how a part is mated.

Timelord

 

[dogarila]

MattP, your suggestion would be very helpful. Often I experience exactly what you're describing above. Sure is good to rename your mates but an assembly can have hundreds and hundreds of mates and renaming them takes time and time is money so...who pays for renaming the mates?

Go ahead and put your enhancement request.

 

[CorBlimeyLimey]

Renaming features, patterns, mates, etc as you create them is the best way to go. Sure it will take a few extra minutes to create ... but could save you or other users hours of searching when revising or otherwise manipulating large parts or assemblies.

It also helps when creating Equations & DT's. See FAQ559-590

from (the City of) Barrie, Ontario.

Everyone has a photographic memory. Some just don't have film.

 

[CorBlimeyLimey]

Also check out thread559-86848 ... it has lots of good tips.

from (the City of) Barrie, Ontario.

Everyone has a photographic memory. Some just don't have film.

 

[dogarila]

How about an enhancement request for the option to give a name to the mate at the time of creation. I mean an extra text box where one can type a name.

 

[SBaugh]

On time of creation highlight and push f2 key. Add your name and click Enter. That doesn't take that long to do.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[CorBlimeyLimey]

netshopo21
Your wish is SW's command.

This feature already exists in SW04. Upon creation of a mate, it's system generated name is highlighted in the "Mate Dialogue Box" ready for renaming "on-the-fly". It remains highlighted until it is renamed or accepted (by clicking on the green check mark) or by starting another mate selection.

from (the City of) Barrie, Ontario.

Everyone has a photographic memory. Some just don't have film.

 

[MattP]

Well naming mates is great but it is still time consuming going back thru a list of mates with names that often don't make a whole lot of sense anymore months down the road. I still think the tool would be helpful for non organized people like myself. Maybe something added to the "Move with Triad" feature.

 

[macPT]

MattP

In the feature manager tree, going down one level, you can easely access a folder with all the mates related to that particular part/subassembly (if you have "view features" selected) or you can have imediatly all mates if you have "view mates and dependencies" selected. I suppose this will help.

Renaming is an art on itself. You must take great care for the names you are choosing. They must be very simple and they should be objectively connected to features or mates so they can be easely identified by another user.

From my experience (for many years I was against changing names, now I am against not changing them) renaming features and mates will help a lot understand the modeling sequence and intent. Editing a model created by someone else or a long time ago will be an easy task. But if you don't create meaningfull simple names, well then maybe it's better not cahnging them at all.

Regards

 

[uncleal52]

For large assemblies, you should be creating sub-assemblies. Its easier to poke around smaller sub-assemblies (and understand what you did) than a model with over 100's mates. Also will help speed up your system, since rebuilds only look at a smaller number of mates and doesn't rebuild your subassemblies every time.

 

[EdDanzer]

We sent in many enhancement requests from 1996 to 1999 about your idea. The comments given by others are what we have got so far.
Don’t hold your breath for more. Suppressing items is quick and will show the general area to suppress individual mates. We have assemblies that are older and it is quicker to do it over than fix the old.
I will spend several hours a week fighting with this problem. Today I could not open a drawing until I closed 16 files, reloaded SolidWorks and opened the file through Explorer. This file was last opened in 2001, and took 10 minutes to open and resume working with the rest of the assembly and drawing pages.
I find working with older assemblies and drawing a real pain.

 

[SBaugh]

Have you used the Conversion wizard on your parts? ANytime you open a older file that hasen't been converted over to the latest version. YOu should expect a slow down in loading times. That's has been the case since the beginning. It's because it's updating the information within the file to the latest version. If you had used the conversion wizard, then it probably would not take as long.

As many problems as you seem to have. Have you tried making a new profile to see if that helps some of your issues?

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[EdDanzer]

If an older SolidWorks file will not load correctly manually, the conversion wizard will not open it and resave as an up dated file. If the file opening caused a lock up, rebooting will be required in the conversion wizard. Another drawing file saved in 2001 that was created in 97 did the same thing yesterday. Another reason we don’t use the conversion wizard is we need to add information to most of the file properties, and would like to see how often a file is updated. The concept of opening and resaving a file every year is a waste of resources, of which we have limitations.

As to mate problems. If there are more than 10 parts in an assembly that have mate problems, take several and create a new subassembly with some and see if you can isolate the problem mates in the subassemblies. Now days we try to limit any one assembly to 20 pieces, maybe 50 if there are a lot of fasteners, so debugging is quicker. The added benefit is faster production of the next iteration. Some of our designs may be changed 5 or 10 times to meet new requirements, just by modifying 1 or 2 subassemblies. This can also speed up making production drawings.

 

[macPT]

Maybe this is out of context, but since it was referred by EdDanzer, I will write about it.

I always convert all the files to a newer version. I think that the conversion wizard pretty robust and it can be left working for the night. Files with errors will be skipped. This way there's no resource waste to do the conversion.

There's always half a dozen of files that, for one reason or another, where not successfuly converted. Normaly this will take less than one hour to correct.

The conversion is made on a copy of the database. The new files are used after some tests. A backup of the original databese is saved (we never know what can happen!)

Regards