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This will be The death of me..

L

LT72884

New member
This program is driving me NUTS. I just started using it last week. My professor said he would be teaching us but never takes us to the lab. he reads us the book and says go home and do it.

So i have been following the rodger toogood tutorial book and i can do the excercises but some of the things i want to try, i cant seem to do.

For example. i have a square block. In the middle of this block i have sketched the letter "U" and then i try to cut the material away but it says unattached extrude. I assume it says this do to the fact that there is no connecting line at the top of the "U". If this is so, how do i create a line that will connect the two points at the top of the U together and extrude both sketches as one? I can draw the line as a second sketch but when i try to extrud both sketches, it hates me for it..


also, how do i move a piece of the part around? IE, i have a part that looks like a fan and i want to free move one of the blades around to alighn it the way i want to?


thanx
 
The problem you're having is you are trying to exturde a solid with an open sketch. Depending on what you want to do you have a couple of options. If you want to remove material in the shape of the U you need to select some more of the icons the Remove Material and Thicken Sketch icons within the extrude feature. If you what to close the sketch you need to edit the existing one and add the line to it, you don't want two sketches.


As for your other questions it sounds as if you have some experience with other 3D modeling software? If so what because ProE is probably not going to be the same as to what you are use to?
 
Google sketch up and blender 3d modeling. I have used sketch up MAYBE 3 times but it was simple. hahaha

blender i used once but that was it so it dont count. haha

SO im not understanding what pro e is then if its not like other 3d software?

How can it be this popular if it is missing such basic features such as moving parts?

So i need to edit the existing sketch rather than merging two sketches into one? OH MAN, how do i edit an existing sketch?

Also, the hole reference plane and sketch plane is anoying. when im in sketcher view, i cant tell whats what. it looks like a piece of paper with a graph drawn on it that says top front and right. But when i draw my picture, it always comes out upside down....

thanx guys, i really appreciate it
 
LT72884 said:
SO im not understanding what pro e is then if its not like other 3d software?

How can it be this popular if it is missing such basic features such as moving parts?
Click to expand...
Pro/e isn't really intended for non-functional, purely aesthetic 3d modeling - like character animation or 3d graphics for a music video. Its more catered toward the modeling of products / items which are to be manufactured by a particular process. As such, things can't just be dragged around to approximate, 'oh it looks okay there' positions. Things need to be placed with intent, which is why dimensions and constraints are used to place something.

So i need to edit the existing sketch rather than merging two sketches into one? OH MAN, how do i edit an existing sketch?
Click to expand...
In your model tree, select your sketch feature, right-click, Edit Definition:

View attachment 4710
 
The reference plane is something that gets many first time users. It's used to orient your sketch. In other words, which was is up?

When you pick a reference plane, you're spinning the sketch so that plane faces the direction you specify. So, it you pick 'TOP' in the direction drop down and then pick a datum plane named DTM1, the front side of that datum plane will face the top. So which side is teh front? If you spin your model you'll see that one side of your planes is brown, the other is gray. The brown side is the front side. So, then Pro/E will orient your sketch so DTM1 faces up or to the top.

I've heard good things about those Toogood books, they should cover all of this. I've used Sketchup quite a bit. It's a decent program, but a lot different that Pro/E. One of the big difference is that Pro/E is feature or history based where Sketchup is a direct modeler. In other words, Pro/E keeps a history of how the part was made and uses that history as an instruction sheet to build the part or assy. To change the part you change the instruction set. In Sketchup, you simple modify the solid as you go, like forming clay. If you want to change things, you just change them.

There is a lot of power in both approaches. The history based method takes a lot more deliberation and thought, while the direct method can produce results quickly. I think ultimately the history based approach holds a lot more power for capturing exactly what you want, and changing it, once you master it.
 
holy crap.. lol..

The toogood book is ok but doesnt really explain the planes to well. I read that chapter 3 times and i still have no idea what he means. He uses words that i have to google because they are words that i guess have stuff to do with 3d stuff. Like constaints and tangents and fillets and 3 point tangents. never heard of those words before.

All he says is that you see the words top, right and front as your directions that reference to the screen. Well, if i go into sketcher mode i see top on the right bottom side of the screen and front on the left and right on the bottom so when i tried to draw something, it was all sorts of messed up. I followed the book and made sure i grabbed the correct edge and refernce plane but still all messed up.

The pic below shows what i mean. That picture means nothing to me because i cant tell what it means.. I understand that things have to be exact because its building parts but this is confusing. oh well,, i still have to learn it so i might as well buck up and learn it..

I tried to grab the right side of my object wehich was a circular edge and it would go into sketcher, something about an illegal move because its a curve????? That curve is my right edge..

thanx guys

sketch_plane.jpg
 
Thanx for the link. i will read it tonight as i do my homework for my design class. Sorry if it seems like im being eragant or rude, but this program is not at all like others i have used.

Thanx for the help guys.

Ill post a pic of what is going on with me with the extrude remove material. For example, i can cut a u shape out of a single block but if i build another block ontop of that block and try the exact same cut on the second block, it says unattached extrude.. ill post a pic. thanx
 
For the planes you can change the colors if you want to make the two sides stand out more. You can also tell the sides based on the coordinate system. With the standard start part the positive side of the planes point along the positive coordinatedirections (X, Y, Z). Here are some screen shots of the planesusing the pre-wildfire color scheme (yellow -poditive side, red - negative side (looking at RIGHT plane along the X coordinate direction)):


View attachment 4717View attachment 4718


In relating these to the predefined views RIGHT (+X), TOP (+Y), and FRONT (+Z) are views of the positive (yellow) side of the planes and are labeled RIGHT, TOP, and FRONT in the view manager and Named View List. The RIGHT (-X), TOP (-Y), and FRONT (-Z) are views of the negtive (red) side of the planes and are labeled LEFT, BOTTOM, and BACK.


When you define a sketch you specify the sketching plane and a direction to orient your sketch in a 2D view. When you select the sketch plane you see an arrow which indicatesyour viewing direction. Here is a picture of what you see:


View attachment 4719


From the picture the sketching plane is the FRONT plane and your sketch will be created viewing the positive side of the plane. The 2D viewis oriented so the positive side of the RIGHT (+X) plane points to the right side of the screen and the positive side of the TOP (+Y) plane points to the top side of the screen as seen in this picture:


View attachment 4720


Notice the coordinate system, Xpoints to the right, Y points up, Z points towards you. In picture 3 if you were to choose a different orientation for the RIGHT plane picture 4 would update accordingly (ie choose Top and notice picture 4 is rotated counter clockwise, Y points left, X points up, Zpoints towards you). Another thing that can get you confused is if you where tochange the viewing direction. If youlook at the negative side of the FRONT (+Z) plane and keep the orientation for the RIGHT (+X) plane as Rightyou would see a red outline for the FRONT (-Z) plane, RIGHT (+X) points to the right side of the screen, and TOP (+Y) points to the bottom of the screen. Notice that X points right, Y points down, Z points into the screen. Here are some pics showing how changing the viewing direction reorients your sketch while keeping the RIGHT (+X) orientation the same:


View attachment 4721View attachment 4722
 
Wow, thanx for all te info and pics. im still having troubles understanding the reference plane. I dont see why it is needed. I see from the pic that the sketching plane is the front plane which i understand, but why do we need a reference plane? To me all i need is one plane wich is the one im goign to draw on. To me, when you say sketch plane is fron but reference plane is the right. it means the image is going to travel to the right which in fact it doesnt because if i use the extrude tool, i pull it towards Z not X..

OR are you saying it will draw the object on the right half of the plane? As in, if i draw a box in the top front area( top right quadrent of pic 4) the box will travel on the + right side and front of the planes like i have outlined in my pic below

referance-plane-ex.jpg


Thanx. After this question i will post more pics of my problem with cutting. but i think im understanding now.

thanx


Edited by: LT72884
 
You need it because you are defineing geometry in 3D space. Here are some pictures of what happens when defining in 3D space and you change the view direction for the section. First two viewing from the FRONT (+Z) with orientation RIGHT (+X) set to Right.


View attachment 4723View attachment 4724


I know it's hard from the picture but notice where the sketch is located with respect to the coordinate system. Now the second two viewing from FRONT (-Z) with orientation RIGHT (+X) set to Right. If you were to ignore orientation you would sketch in the upper right quadrant as in picture 3 to make it the same as picture 1. Notice where the sketch is located with respect to the coordinate system in picture 4 and compare to picture 2 if you assume orientation doesn't matter.


View attachment 4725View attachment 4726


If you ignore orientation you can end up placeing geometry where you are not expecting it to be.
Edited by: kdem
 
hmm, ok. i will read over your info, but what i would like to know is if i was on the right track with what i posted. The red outline, to me, is where the box in the below image will be drawn.

View attachment 4727

from this picture above, i gather that the image will be dranw in the area marked off by my red outline below since those are all in the positive direction. So to me, the box will exist above the top plane(y+) and to the right side of the right plane(x+) and in front of the front plane (z+). If this is true, i still dont know which one to pick in relation to my sketching plane.

referance-plane-ex.jpg


Thank you all for your patience and time. I understand it must be annoying to answer my questions. haha


Edited by: LT72884
 
You are actually drawing in a quadrant on the front plane between the postive right and top planes (first quadrant x-y-z cartesian coordinate system)


View attachment 4729


The right plane is only a reference for orientation and for location.
 
Think of it this way.

You sketch plane is like a piece of notebook paper, with the holes along the side. You can sketch on it anyplace you want, but you can also turn the paper any way you want. The holes can be on the right, on the left, the top or the bottom:

View attachment 4730View attachment 4731View attachment 4732View attachment 4733

The reference plane tells Pro/E when way to turn the paper. You pick a plane that's perpendicular to the sketch plane and tell Pro/E which way to point that plane so your 'paper' is turned the way you want.
 
If you pick the FRONT as your sketch plane from the images you have two choices for references RIGHT and TOP. You can pick either one but you still need to understand how the orientation affects where your sketch is placed and how things in the sketch will be oriented. If you chose FRONT as the sketch plane and RIGHT setwith an orientation to the right and draw in the upper left quadrant you end up with this:


View attachment 4734View attachment 4735


If you chose FRONT as the sketch plane and TOP as the orientation planewhen you ignore orientation you would leave TOP set to the right orientation but notice what happens to the sketch. Not only is your geometry in a different quadrant but it is also rotated to a different orientation.


View attachment 4736View attachment 4737
 
Hmm, very interesting indeed. So if i were to take this image:
and then rotate it 90*CW, it should end up at the same points as the first image correct. I think im begining to see how it all works. Once i outlined my image with the red line, i could see thats where the box was going to be drawn. Im going to have to print this thread out for reference. im just going to have to visualize in my head before i draw the object i guess.



View attachment 4738


thanx guys. Oh and the paper analogy worked to. I thought bout this
last night and i was trying to compare it with a piece of paper but
never thought of the holes.. hahaha. Ok, now onto my next question. Do
i need to create a seperate thread for other question or will this one
work.



thanx



Matt
 
LT72884 said:
Hmm, very interesting indeed. So if i were to take this image:
and then rotate it 90*CW, it should end up at the same points as the first image correct.
Click to expand...


That's correct.
 
kdem said:
LT72884 said:
Hmm, very interesting indeed. So if i were to take this image:
and then rotate it 90*CW, it should end up at the same points as the first image correct.
Click to expand...


That's correct.
Click to expand...

good. i was hoping i was correct. now i have to remember all this. I now understand refernce and sketch plane. next i get to figure out how orientation option works with it all. I read the above posts again and when im off work, gonna play with pro e a we bit.

thanx
 
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