Managing Relations in SW: Jumble of Messiness 3

[rokahn]

I've been learning SW for the past month and gone through a lot of what other people probably go through and after having to start over designs many times, I'm concluding that SW doesn't have a reasonable toolset for managing relations (unless I just haven't discovered how to use it yet).

For example, I based some sketches off a base feature sketch which turned out to be unnecessary. I tried to remove this base feature using three different approaches:
1. I tried to use the Sketch Relations Property Mgr to track down relations to this base feature and delete them but it was very difficult because SW doesn't indicate which sketch owns the entities associated with each relation--is it in the undesired base feature or in another sketch?
2. Next, I tried to delete the entire base feature but all the dependent sketches totally disappeared.
3. I removed all external relations (causing most entities to become undefined) and then deleted the geometry from the base sketch. At least the sketches didn't disappear entirely. But then I was unable to delete the (empty) base feature because one can't delete a base feature...or reorder them. If I copy a useful sketch into this base feature, the remaining relations disappear (in addition to the relations which disappeared when I deleted external relations)
...time to start this part over.

After experiencing a number of problems like this, I'm getting farther along each time (give me another 2 months and I might be useful) but the lack of tools to visualize and edit relations cause me to become more and more conservative/rigid in my approach to using SW. For my next attempt, I plan to make one base feature with just a few construction lines in it that are needed in more than one sketch so that I don't have to edit the base sketch much or reorder/delete it. SW seems very far from being able to capture a creative stream of design decisions and manage them as changes are necessary. Is it necessary to plan out where to embed all the global datums before starting the design? This is a much more structured approach than the tutorials seems to suggest.

Perhaps I've not been making full use of the Sketch Relations Property Mgr...or maybe this is an inherent limitation of the current generation of parametric CAD applications. Any views?

 

[rokahn]

Without igniting a religious war please, are there other CAD apps that manage relations better (e.g. ProE or Inventor)?

 

[SBaugh]

When you make a Base extrusion. 99% of time all your sketches from there forth are based off that extrusion. If you don't want that to happen you must learn to use Planes for EVERYTHING. If you just use and edge, a point, anything about it you have now created a relationship to the base extrude. I have found ways (depending on my Design intent at the beginning) so that I could delete the Base_Extrude without deleteing anything else. "Try that!" ;-)

To figure out sketch relationships you can turn off the automatic relationships or keep it on don't matter as long as you know what your doing. I keep mine on, because if I place a line in my sketch and for some reason it makes itself coincident to an edge or something. I then place a dim to it and change the length to X.XXX. The dim is going to cause an Overdefined mate. Well to fix the problem I would just say make the dim driving (or you can set it as a default to answer that question "yes" make it driving). It would then turn red and I would first pick the delete relationship icon. I would highlight the line. If that didn't show a red coincident in the PM (Property Manager) window I would start picking points. It can only be those 3 things causing the problem. I find the red mark and delete. Sometimes I have had up to 3 or more problems but once I found it my sketches were fine.

I hope your using fully defined sketches before you exturde them? If not, then you can so many problems later down the road, that I don't think my typing hands could answer all of them ;-).

If your having trouble with assembly mates:
Learning assembly mates I would say is one of the hardest things to pick up in SW. Repairing Mate problems is the next hardest part of SW. But with the SW today it is a WHOLE A LOT easier than it used to be. Now when you get an error in the mates, it gives you the Cherries showing the problem Mate or Mates and they give the Yield looking sign showing you the mates that are affected. You have to learn what those symbols mean. You also have to learn how to simply Suppres the mate VS deleting mates. Once you learn that repairing and making mates are a snap.

But what all this boils down to is "Design Intent" The way you make it in the beginning, well determine the entire job, and that is the way most all of todays CAD systems are about.

I hope that helps you and others, Scott Baugh, CSWP
credence69@REMOVEhotmail.com

http://www.3dmca.com

http://home.insightbb.com/~scott.baugh/

*When in doubt always check the help first*

 

[aart2]

When you start a new part, you will always need a base feature. If you come to a point that you want to change the way the part file is defined, you will have to reconsider all kinds of features. When you collapse all features in the feature manager tree, you can start by editing your base feature or the sketch of the base feature. After all you will always need a base feature, so: why not edit it?
After this you can drag the border of the feature manager over the previous defined features (one at the time, in order to check if all relations are still OK, if not, you can restore them in the way you want to have them.)
I always use very simple sketches, I much more define a geometry by using a lot of features. This makes it more easy to define relations (sketch-tip: use the sketch tool 'convert entities' whenever you can.)
This method gives me a great deal of freedom in designing.
It is true that after designing a part I sometimes have big files, because I define several design solutions using configurations. So after this stage, I usually make a new part in which I can define the right design in the most effective way. Maybe this seems like doing it twice, but in my opinion it isn't.
In the designing fase, I want to be flexible using all kinds of features I want to manipulate and/or suppress. While in the final definition fase, I want a comprehendable no-nonse part, which is easy to handle. This part is easy to define, since you allready defined it's geometry in the designing-fase.

I hope this is useful for you. I remember my first weeks of solid modeling, and it was no fun at all because of the many things that I didn't understand. But now I'm working with SW for a year and I really feel comfortable with it. You will always need some time to get into new things(like solid modeling). And after all: a month isn't very long yet.

 

[BBJT]

rokahn,
Don't feel like you are alone. SBaugh did a great job replying to your question. I know I could not have answered it better. The question is where did Scott obtain this kwowledge? I am guessing the same way I did and you will. You stated that you are getting further along each time. That is the key. You learn from your mistakes, or SWs mistakes(limitations, and use it to your advantage in your next model. Please make sure you enter your ideas and pains in as an Enhacement Request.

All the packages are the same when it comes to this topic. With enough Enhancemnt Request it can only get better.

Godd luck! BBJT CSWP

 

[BBJT]

By the way the last post ended off with a typo. It should have been GOOD luck! BBJT CSWP

 

[rokahn]

Thanks for all the comments...you've given me new hope.

There seems to be a split in the design philosopy.

Scott Baugh advocates sketches sharing few if any relations.

Aart2 keeps sketches simple but highly interrelated ("use convert entity as much as possible&quot and keeps most complexity in the features rather than the sketches.

I'm beginning to think there's no one "best practice"--it's just knowing how to get 'round the limitations of whichever practice you practice. I've been drafting complex sketches with minimal content in the features. The complexity allows me to have fewer sketches but it's harder to track down relations because of all the entities. I've been using convert entity frequently between sketches. If this particular combination is not advised, please let me know.

Is it better to make the base sketch very simple or to put a lot of the complexity into that sketch? (Or maybe either solution has proportional tradeoffs.)

Scott, how do you tend to portion out design complexity between sketches and features?

 

[SBaugh]

Complexity of sketches in my opinion is bad. It makes it hard to see how things were done espiecally if someone else has to come in and see what you've done. I feel it is better to make adequete sketches, but not so they are complex. So my opinion don't make real complex sketches, things will go easier on you down the line if the sketches are more simple.

As for Converting entities thats fine, but if something changes well that sketch is esstenially going to change to fit. This is a common practice for Automation. I like to make most of sketches as individuals. I don't convert enities that often unless I can foresee that it will not be a problem (Never can tell sometimes though). If my sketches are going to reside on a edge it gets a Colinear relationship if I already placed the line in or I will convert the entity if I have not already placed a sketch line in. Just depends on the situtation.

Does that help? I'm a bit slow today...under the weather a bit.
Best Regards,
Scott Baugh, CSWP
credence69@REMOVEhotmail.com

http://www.3dmca.com

http://home.insightbb.com/~scott.baugh/

*When in doubt always check the help first*

 

[BBJT]

Simplified sketches make it a whole lot easier for trouble shooting and for modifications down the road. For a simplied example...if you want to remove a fillet or a chamfer it is much easier to delete a feature than it is to go into the sketch and remove them. Removing them from a sketch, you may find yourself spending extra time re-fully defining that sketch. You can also suppress features. If it is a sketch feature the only way to remove it is to delete it from the sketch. BBJT CSWP

 

[SBaugh]

Thanks BBJT!! You explained it better than I could today...and you did it with a whole lot less typing than I. ;-)

Best Regards, Scott Baugh, CSWP
credence69@REMOVEhotmail.com

http://www.3dmca.com

http://home.insightbb.com/~scott.baugh/

*When in doubt always check the help first*