solids (from a surface guy)

[Barry]

I've been surfacing for 5 or 6 years. I have v8.1.1 and bought solids with it. Im on my 5th job using solids. Its alittle more complex ( somewhat small detail). I am having trouble with fillets and corner radii. I can't seem to get them to work in quite a few areas. .125 fillets and .06 corners. I know I can do it in surf but i dont want to give in. Please advise

Thanks,

Barry

[cadcam]

Well I don’t know were to start, there can be many resins.

do you have a file that you are having trouble with so maybe I can see were the hold up is by the shape restrictions.

[Kenneth Potter]

I feel your pain dude

Making the transition from surfacing to solids is not that bad when you understand the rules . I suggest you get the mastercam solids tutorial .That will get you going on the basics.

 

Kenneth Potter

[Guest CNC Apps Guy 1]

James Meyette's Rules for Solid Modeling:

[*]Rule # 1 - Draw your geometry sharp.

[*]Rule # 2 - Fillet edges faces, etc...

[*]Rule # 3 - Drag the Stop Operation around in the Solids History Tree instead of using "Supress".

[*]Rule # 4 - Thou Shalt be patient when learning solids.

It is a different beast, bound by more limitations(mostly mathematical from my understanding of the process) than surface modeling. There is a reason why Automakers/Airplane Mfr's etc... use software like CATIA®, Alias®, and not Solid Works® for designing body panels, fuselages, etc.... The reason being that freeform/organic shapes are much more difficult to create using solid modeling than surface modeling, so you may find using a combination of both may acually suit the types of parts you are creating.

JMHO

[ 11-15-2001: Message edited by: James Meyette ]

[KMaynard]

OK James,

I'm a little green on this one .don't flame me too bad.. Why use the stop option over the supress?

Kev

[ 11-15-2001: Message edited by: KMaynard ]

[Barry]

Thanks for the replies. I did go through the solids tutorial book if thats what you mean. I did build all sharp to start. And by the way I love the initial building of the part(very fast) and minimal geometry. When it came to filleting things slow down considerably over surfacing. Of course it could be due to my inexperience. The thing that puzzled me was I have some areas that are symetrical, one boss would fillet perfectly, the other one wouldn't. Both bosses intersect the body in exactly the same way. It just doesn't make sense in my little head!!! I am being patient, I started over trying a different area as my main body. It didn't make much difference. Soon I will have to bow down and finish in surfaces, which I thought was an evil act, but after reading your responses I guess it is an accepted weakness. I thought that solids was that magical solution to all our designing problems. I am sadly mistaken.

[Barry]

yeah the stop option I forgot to bring that up. How does it differ?

[gstephens]

Fillets are the trickiest thing to deal with in solids. You alsways have to be aware of the "Faces" that actually define the solid. To get an idea, look at the solid in wireframe view (hide all the rest of the geo).all of the lines/arcs you see are edges of faces. The biggest thing to remember when filleting is that you CANNOT cause a face to disappear. If you have a sliver of a face, and you try to fillet an edge next to it, chances are it will fail. Sometimes you can get around it by re-ordering your operations. Sometimes if you use different base geometry (lines and arcs instead of splines maybe or vice-versa) you will get different face definitions for the same solid model. Try using a minimal (.001) fillet radius on a problem area, then gradually increase it until it fails. This is a good starting place for finding out if you can even fix the problem. All of these issues are limitations in the solids kernal (which by the way is the same one in UG and Solidworks) which is getting better all the time.

Stop-op instead of supress is a good idea for two reasons. First and foremost, it's usually faster. Second, suppress is dangerous in that if you add a feature after you supress something, the edges/faces that control the supressed op may be altered which causes the op to be marked invalid. The downside of stop-op is that it will not remove an op out of the middle of the tree, just the end.

[Mark H]

Barry, I also have had problems with filleting in solids, so your not alone. As gstephens pointed out, its a little of trial and error. If I cant get something to fillet, I just change one of the settings. For example, try using the tangent option - propagate along tagencies and select only one edge, or do not use the tangent and select all of the edges, or select only a face... I think you see where I'm going with this.

But it is strange how one feature will fillet and another will not. (And the features appear to be exactly the same.)

[ 11-15-2001: Message edited by: Mark H ]

[Kenneth Potter]

Did I hear someone say"""" Alias""""

 

Free Form Rules

Solids can be used to create your most simple shapes Really Really Really Fast. What i do alot is explode those solids So i can get parent surfaces to build from & work around """ Seamless water tight edges dude

 

Kenneth Potter

Mastecam Version "10 " Enthusiast

[ 11-15-2001: Message edited by: Kenneth Potter ]

[Scott Bond]

Hi

I use most of the moves that have been mentioned here.If starting with a smaller fillet didn't do the job,try to draw the void as a separate solid then use remove.

"I know I can do it in surf but I don't want to give in."

Sometimes I have to go all the back to saving nci as geometry,edit out the cuts I don't like,and then resurface the part.

"Please advise"

I try to avoid the hobby side of modeling - before my real commitment ,to make part correct and on time.

[ 11-15-2001: Message edited by: Scott Bond ]

[Barry]

thanks to everyone for your help. Most of the things mentioned I have tried in one form or another. There seems to be far less "escape routes" with solids than with surfaces. I guess that was touched on by a few of you guys. This is not a surrender mind you. I will continue to fight! Thanks again to everyone. I think you will see more of me on here in the future...I mean see me on here more..that sounds alittle better.

Barry Hansen

Brillion Pattern & Machine

CAD/CAM

peace, harmony and high speed machining to you all!

[Simtech]

Hi All ...here's my 2%

In some cases, you can resolve filleting problems by creating the opposite of the part. If you are modeling the core of a part, throw it in a block form and remove it to get the cavity.

Now in the cavity part, it's easier to get the radius or fillets to work because you actually add material to the solid, while when working with the core you are always removing material from the solid part.

A lot of us have been patient and tried many many ways to get around filleting problems.

My last recommendation: make the filleting portion of the job the last thing you do, if possible.

Even with the headaches that solid modeling does create, many times it's way much easier to work with then in surfaces. Keep to it! Practice makes perfect .... and you still have surfaces.

BTW, V9 is coming up with a lot a very interesting stuff for solid modeling!

Luc

[cadcam]

Well I can see I was no help.

But go with what these gentlemen have said.

Some time when a fillet gives me trouble I try change the sequence of order of how I built the model.

I have this problem yesterday.

Changed the order and it worked great.