solidify problem

[Checkmate]

hi, i have been trying to use solidify to cut from a solid using a surface as in the pic below,

but when i press the green tick it fails and says "WARNING: One-sided edge found in CUT." like below. as far as i know all of the boundaries where on the surface of the solid but i'm guessing this is not the case. like in all the othe boundaries the boundaries are sketched curves that i thought were on the surfaces.how do i sort this out? thanks

thanks,

 

[deepakbhat_nie]

Hi,


Extend the surfaces at the outer edge and give a try it should work.


Regards,


Deepak Bhat
Edited by: deepakbhat_nie

 

[Checkmate]

cheers, i'm asuming you meant extend, i tried selecting the surface or the edge but extend seems to be blanked out. what should i do now? also the surface i am using to cut with was made in style and is joins tangetially to the surface that is causing the fail.





thanks,
Edited by: Checkmate

 

[deepakbhat_nie]

Hi,


I am sorry for the spelling mistake.Yes I ment extend.just create a surface at an offset from DTM1(shown in the pic say5.00 mm) .to select the edge select geometry in tree filter and select the edge of the surface.now click on edit extend and select extend up to surcace option(second icon on the bottom left corner) select the datum plane which you have created by offsetting the dtm1.GIVE A TRY I THINK IT IS WORTH IT.if you can upload the part we can give a try on the same.


Regards,


Deepak Bhat
Edited by: deepakbhat_nie

 

[Checkmate]

thanks,


when i select the surface and then select the edge, i am not able to select the extend in the edit menu, also perhaps i should tell you that the surface is the result of two surfaces merged then the new surface mirrored and then merged again not that i think that should make any difference, but i coppied all the boundary curves/ edges (i'm not totally sure which they are or how to tell) into one. unfortunately i can't post the file because it is done in a student version so is not compatible with most other versions. have you got any other ideas of how to go about it?





thanks,

 

[dojo]

Hey m8,


Extend will never work as all sides are tangenten the extension in vertical direction will result in the surface curling inwards into the part.What gives you a clue is that the patch icon is blanked out. In this case you should be able to to select it on the condition that all edges of the quilt lay on the solid so recheck all your curves, and also recheck the tangency direction so there is no curl in your surface


I do not understand the part 'surface is the result of two surfaces merged then the new surface mirrored and then merged '. Normally would have created a single side of that surface, mirror it and merge. To create the same shape on the other side of the model you then mirror this whole quilt. So in you explanation there is one mirror 2 much?


Try to change the accuracy, but i doubt seeing the model size that this will be the solution. goto 'edit' 'setup' 'accuracy'. Change the relative to absolute and set the value to 0.01. See if you can create the cut then. Ill have to check 2morrow but I think in the model I've made there wasn't a issue with the cut? (cant remember)


What you could try and do is copy the surfaces from the solid where the cut needs to be (the two surfaces from the torus, and the two surfaces from the lil 'mouth'. Make a intersection curve of this copy with your surface you want to cut away. It should form a closed loop on the boundary, when all the edges are on the surface. Even more you could then trim the copied surface with this intersection curve and try to merge it to the shape surface.


Nick

 

[ctolman]

ProE does not like to trim any surface that comes tangent to the solid it is trimming. Accuracy can fix this but there is another trick! Try building a couple more surfaces that will build a closed box or quilt completely outside of what is currently the solid. ProE tends to resolve quilt cutting issues much better if it is working with a closed volume. It can than realize what should be on one side of your quilt and what should be on the other side!

 

[dojo]

Thats rubbish ctolman, how do you think you create consumer product plastics, cab interiors etc? it has nothing but tangent and or curvature continious surfaces trimming other volumes ....

 

[Checkmate]

yes what i said about the 4 surfaces being merged was rubbish sorry. i went back over everthing i did and it appears that the problem was when i did that extra curve for the style boundary tool, i rounded up the length of the control points. anyway i redid it and this time it worked fine.


cheers for all your help, dojo and deeppakbhat_nie


thanks,

 

[jeff4136]

Actually, Pro/E (or any system) does occasionally have
trouble defining trim lines when merging surfs that
overlap at near tangent. What might be done to correct
it is to copy solid surfs interfacing the new quilt,
manually trim it using new quilt boundaries, merge >
join, and finally solidify the results. I'd also check
that new quilt carefully to make sure it's not dipping
in and out of the solid. You might try creating
intersection curves to make sure the only intersection
is on the boundaries.



* * * *
Can you post the part (what ver) or, better yet, a
STEP containing the solid body and the cutting
quilt?

Edited by: jeff4136

 

[design-engine]

over extend... yes. Think of your cut as a knife
cutting cheese. If your knife does not go all the way thru or over extend
then you have to break the cheese.



Sometimes if you increase the accuracy of your part the coincident surface to
the solid works.



There are several different kinds of extends too. One is a g2 type of
extend referred to as 'same'. The g2 or tangential extend is referred
to as Tangent. There is approximate. I think that is g0 or
positional.



Basically if the same extend does not work try the Tangent extend. If I
were writing the interface I would rename the extend names to g2 - g1 and
g0 or continuous - tangent and 'up to a datum'



Edited by: design-engine