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Un attached extrude

L

LT72884

New member
Ok, so i have screenshots of whats going on. The first pic is of a block i made and then used a "u" shapped line to cut out the center.

View attachment 4741

You can see the sketched line just fine. I extrude it and it works perfectly

View attachment 4742

So i try to create a box ontop of a platform and try to cut out the same shape and i get an error

View attachment 4743

cut-2-un-successful-1.jpg


As you can see, its the exact same line and sketch BUT i get an error... I dont understand why either.

thanx
 
its part of my homework. I must cut a square section out like the first image but on the second and it wont let me.
 
close the section and it will probably work. and make sure that the "line you add" is outside the "topsurface" of your part. Makes it easier for pro/E to calculate , and also a more robust model.


//tobias


View attachment 4744
Edited by: tobbo
 
saravanans_87 said:
LT72884,

i tried & working fine here ..
smiley2.gif


may be u can try it once again....
Click to expand...

i dont know how you got it to work. Remember that i made the long rectangle piece first then i drew the box on top of that and extruded it out and then i tried to cut. its not a single sketch that loooked like an L shape and then extruded out. It one box half the width ontop of the other and then the U shape cut.
 
When you created the sketch did you use the top surface of the block as a sketch reference? In the first picture the top surface wasn't used as a reference (the dashed lines are the sketch references). Although the end points appear to intersect the surface they actually don't and will cause the error you are getting. The second shows the top surface used as a reference.Notice the circles at the ends of the lines on the top surface reference, those are point on entity contraints which contrain the end points to be on the the surface reference.


View attachment 4754View attachment 4755
 
Hmm, i might not have used it as the reference plane. let me check it out and ill let you know, thanx guys.
 
Good description kdem.


still, LT72884 , why do you want to use an open section in sketcher? why not make a closed one , and make sure the "closing line" is outside the geometry? Just be careful how you reference things, otherwise you may get the opportunity to learn more about failuremode :)


//Tobias
 
tobbo said:
Good description kdem.


still, LT72884 , why do you want to use an open section in sketcher? why not make a closed one , and make sure the "closing line" is outside the geometry? Just be careful how you reference things, otherwise you may get the opportunity to learn more about failuremode :)


//Tobias
Click to expand...

I really see your point, i do, but i needed to know why the same cut was working for one object but not another. Almost made me think that Pro e was programmed to be contradictory with new users to just toy with em!!

Im a simple person so when i saw that the same cut could not be duplicated from one object to another,, i freaked out. Oh how my OCD's were just going crazy. Its like having 6 pedals in a vehicle when there are only 4 directions...

i just got out of class so tonight whilst im at home, i will try out all the methods and see what happens. im on chapter 3 of the tutorial book but i am sooo not understanding the concepts.. I swear the book was written for people with drafting exp, which i have NONE. haha

thanx guys
 
"Constrained" means "tied down". What kdem was getting at in his images was that perhaps the top,open ends of your "U" aren't tied down, or constrained to the existing geometry properly. If the top ends of the U don't extend past the top of the block, it's not going to cut it.

I would think that it would fail the feature, not create it and call it unattached. Unless you're saying that you get the error and it refuses to create it.

Unattached sounds more like kdem's initial suggestion, it's creating the cut in the opposite direction and essentially cutting air.

Also, check to see that you have the "cut" icon picked on the feature dashboard and not "protrude" or "surface".
 
dgs said:
"Constrained" means "tied down". What kdem was getting at in his images was that perhaps the top,open ends of your "U" aren't tied down, or constrained to the existing geometry properly. If the top ends of the U don't extend past the top of the block, it's not going to cut it.

I would think that it would fail the feature, not create it and call it unattached. Unless you're saying that you get the error and it refuses to create it.

Unattached sounds more like kdem's initial suggestion, it's creating the cut in the opposite direction and essentially cutting air.

Also, check to see that you have the "cut" icon picked on the feature dashboard and not "protrude" or "surface".
Click to expand...

hmmm, i have the cut going threw the block because i hit the flip icon. I made sure solid was selected as well as remove material and as soon as i hit verify, the error pops up.. When i tried to make the U cut, it wouldnt attach its lines to the top of the box. Is there a way to force a constaint? thanx
 
To have constraints applied when you are creating geometry you need to set the sketcher options. Select Sketch>Options and on the Sketcher Preferences dialog box select the Constraints tab and select the contraints.


View attachment 4758


If you already have created the geometry you can still apply the constraints by selecting the Constraint icon or selecting Sketch>Constrain. Select the icon on the second row and third column. The following pictures show what to select. If you are using WF5 you won't see the the following 2 pictures because there are idividual icons for each on the sketcher palate and menu selections for the main menu.


View attachment 4759View attachment 4760
 
Kdem, thanx for the screen shots. i am currently using school edition 4.0 because 5.0 wouldnt get passed 1% so i used 4.0. With the above pictures, this will allow me to tie down a line onto a NONE referenced line or whatever it is?

thanx
 
ok im back. So im not figure out the constarint thing. With the unattched u cut i was doing, how do i tie down the ends of the u to the single non dashed line?

thanx
 
You can make the top surface a "reference" for constraining. You can do this by selecting the surface as a reference for sketch orientation:


View attachment 4770


Your sketch should then have this surface as a ref:


View attachment 4771


If you did not do this, you can still select the surface as a sketch reference using:


Sketch>References...


View attachment 4772


Then you can snap to that reference/surface/line in sketch:


View attachment 4773


It is never a good practice tocreate sketched features outside/beyondthegeometery. This was a common practice with old CAD systems before parametric modeling.


An open sketch will allow you to cut everything above that open sketch but the open sketch must be constrained to an edge or surface so that the feature can be fully defined and created.
 
dang, thanx for the detailed response. im gonna try it out. I was under the impression that you could tie down lines to non referenced lines. Im still getting used to all of this. haha

thanx
 
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