2D Drawing included

[andrei2]

Hi everyone

For the university project I have some smaller 3D model to do from given (as a definition of the project) 2D drawing. This drawing is included below and so is screenshot of the 3D model from where I cannot go ahead, even if is really basics of proe. If you compare the drawing to the model, its obvious something is really wrong - very huge mistake (probably a way way too much air in the model) but Im trying to go back to the Sketch window (inside ProE). Im afraid I cannot do any more changes (so will need to start everything again) because in the Sketch window is now 3D model instead of 2d sketch as it has been before I pressed on the green tick icon to leave sketch mode. If someone could please assist me what to do next to try to correct this, I would appreciate a lot. Thank you for any reply.

 

[sip]

You are just starting out with ProE?


You must model this with separrate features, similar to a machinist. First extrude the rectangle to the desired depth, and then create as separate features the holes, cuts, and rounds last. Extrude can be solid, and can be changed to cut.


Sip

 

[kdem]

For starters don't try and model everything in a single sketch. Start with an extrude for the overall part. Use the hole tool for the holes or you could also create them using extrude. Create the hemispherical cut using a revolve. For the pocket you could create this as one or two features using an extrude depending on how you setup the sketches. Its a little hard to tell form the drawing but you could probably use the draft feature angle of the side or you might want model it some other way. You could model the cut thru the pocket as part of the pocket or as a separate feature depending on how you want to model things. Add the chamfers and rounds last.

 

[andrei2]

sip actuially yes im starting. Well I have had it for a while on my hard drive but im not so good with creating models from 2d drawings (as i showed my) because I don't see from 2D how it should be in 3D. I have had some experience with given 3D model and trying to do it but really basics. I don't have only one rectangle as you said and from the downer part of 2d drawing, it makes no sense for me how far the depth should be. Somehow I need the third dimension of the main rectangle (dimensioned with B on the right side and with A at the top) but its not definited. Which rectangle did you mean? I know where the icon Extrude is but Im afraid this won't be enough. I have to get normal main rectangle first so I can cut something inside it.

kdem I don't know how to put together sketches. Its too much work for this so Im trying in one sketch only. What do you mean with ''overall part''? Hole tool is hard to use and Im also not sure where it could be located. I would need to define (in the screen after using green tick icon to left sketch mode) the points where the holes should be located but this is really hard. Is it possible to just use circles instead (you said extrude is fine)? However as it is visible in the right upper and downer side of 2d drawinng, I need to use 2 circles (above and below) but there is some icon near the Circle one to use another circle inside already sketched one. Circle is easy to do. Also what is ''part of the pocket''?

 

[sip]

Please take some elementary training, as that is what you really need. The software can be daunting, but this is not the place to train people, but to help when they have a problem. You can start by taking the cell phone tutorial, or you can look here: [url]http://www.sharptechdesign.com/Tutorials/ProE_Fundamentals_W F2/WF2_TOC.htm[/url]


If you have questions along the way, don't hesitate to ask.


Sip

 

[sip]

[url]http://www.ptc.com/products/tutorials/wf4/toc/intro_tutorial .htm[/url]


[url]http://www.ptc.com/products/tutorials/wf4/tutorial1/index.ht m[/url]


[url]http://www.ptc.com/products/tutorials/wf4/tutorial2/index.ht m[/url]


[url]http://www.ptc.com/products/tutorials/wf4/toc/intro_tutorial .htm[/url]


[url]http://www.ptc.com/products/tutorials/wf4/toc/intro_tutorial .htm[/url]


[url]http://www.ptc.com/products/tutorials/wf4/tutorial5/index.ht m[/url]


[url]http://www.ptc.com/products/tutorials/wf4/tutorial6/index.ht m[/url]


These are all on the introductory page of the PTC website: http://www.ptc.com/community/proewf4/start.htm


You may need an account to access them.


Sip

 

[kdem]

Is this part of an introductory CAD class you are taking that uses ProE? If so, the instructor should be providing training materials in some way that shows you how to model in ProE. Ifthis ispart of some other type of course it may be assumed that you have the necessary CAD experience to use the software. It also sounds like you don't have any drafting or engineering drawing experience. The two rectangles as you refer to them are two views of the part. The views are a top view and a front view that is sectioned to show the internal features. The simplest way I know to try and help with visualization in the current context is take a box in your hands and look at it from the top. This would be the upper view in your drawing. Rotate the box in your hands so the top is pointing away from you. This would be the lower view in your drawing. So the dimensions for the outer rectangle are A (length) andB (width) from the top view and L (depth) from thelower (front) view.


As Sip stated you need to look at the drawing and determine the types of features and how you can model them. When I say overall part I mean the part and all its features. With an extrude whatever you have on the sketch is going to be extruded to a depth you specify.Since you have multiple sketch loops (circles for the holes and rectangles for the cuts) ProE will try to add or remove material between the sketch entities. To change the surface extrude you have to a solid select the extrude feature in the model tree so it is highlighted, select the right mouse button, and in the list select edit definition. You should see a dashboard for the feature definition. Above the placement tab there are two icons. One looks like a surface the other a solid. Select the one that looks like a solid. You should see removed materialbetween theinner rectangles, a hole where the hemisphere should be,andremoved material between the circles at the hole locations. To edit the sketch select it in the model tree to highlight it, select the right mouse button, and in the list select edit definition.Try removing one of the inner rectangles and one of the circles at each of the hole locations. This time you should see three circular holes and a rectangular hole. Going back to the drawing you should be able to see that you can't model everything with one sketch. The rectangular steps or pockets as I call them don't go all the way thru so remove the inner rectangle. The hole where the hemisphere should be located doesn't match the geometry so remove it. The holes could partially be modeled since they are thu holes. So the first extrude could have holes of diameter S. The next extrude could be for the counterbores on the holes with diameter V and depth R. Create a sketch on the top surface with two circles for the counterbore diameter. In the sketch select the holes created in the previous extrude as references using Sketch>References from the top menu. This allows you to use the hole centers as references for the counterbore so they are in the right locations. When you create the extrude add material will be the default condition and you should see two cylinders coming from the top surface which is the wrong direction for the feature creation. To the right of the depth value in the extrude dashboard you should see an icon that looks like an angled line with two arrows, select it to flip the direction of feature creation or you can select on the arrow in the graphics area showing the feature creation. Also select the remove material icon on the extrude dashboard. Looks like a sqaure with the corner cut off. Start with this and see how it goes.


Also, you should be able to palce your cursor over an icon in the menu bar and it will tell you what it is.

sip actuially yes im starting. Well I have had it for a while on my hard drive but im not so good with creating models from 2d drawings (as i showed my) because I don't see from 2D how it should be in 3D. I have had some experience with given 3D model and trying to do it but really basics. I don't have only one rectangle as you said and from the downer part of 2d drawing, it makes no sense for me how far the depth should be. Somehow I need the third dimension of the main rectangle (dimensioned with B on the right side and with A at the top) but its not definited. Which rectangle did you mean? I know where the icon Extrude is but Im afraid this won't be enough. I have to get normal main rectangle first so I can cut something inside it.

kdem I don't know how to put together sketches. Its too much work for this so Im trying in one sketch only. What do you mean with ''overall part''? Hole tool is hard to use and Im also not sure where it could be located. I would need to define (in the screen after using green tick icon to left sketch mode) the points where the holes should be located but this is really hard. Is it possible to just use circles instead (you said extrude is fine)? However as it is visible in the right upper and downer side of 2d drawinng, I need to use 2 circles (above and below) but there is some icon near the Circle one to use another circle inside already sketched one. Circle is easy to do. Also what is ''part of the pocket''?

Edited by: kdem

 

[andrei2]

sim thank you for those tutorials. I already have few of them - also, good other ones. You told me that this isn't a place to train people. I know this, thats why I have done the research for tutorials already before. I just wanted to please for assist for above definited (in 2d drawing) project's problem.

kdem yes the model (as the project) is a part of introductory to CAD. We can do this model in any software but since I already have proe installed why not using this. I haven't gotten for this project, any training material. Also not for anything else. The problem is that the drawing doesn't show, or at least I don't see from it, where should be material and where should be an ''air'' (material cut). It would be much easier if I got 3D model and the project would be ''Create the same 3D model''. I knew that upper side of drawing is what I see from the top and downer side is what I see from the front but this doesn't say anything to me.

To edit the sketch select it in the model tree to highlight it, select
the right mouse button, and in the list select edit definition.

I tried this but I still got the model in the sketch mode instead of what I had before clicking on green tick icon.
You mentoined ''sketch - reference'' is this the letter ''A_7'' which is showed on the 3d model? Or its just a letter of an model element? You mentoined ''placement tab'', whats this?
Is in any video tutorial also showed what you tried to type? I see on youtube are many proe - of course I won't find the one with the same model but I might try to find the one with the same functions used as I should use here, in my model. Do you suggest any? Unfortunately (for me) there on the youtube are even more complicated models than my is :'-(


Edited by: andrei2

 

[kdem]

Since you're taking a class and allowed to use whatever software you want to model the part you probably won't get any training material. The front view drawing shows where there is material. Some of it is also drawing interpretation. Asdrafting practice you hatch material that a section plane passes through. So the hatched areas are material and the unhatched areas are where there is no material. The easiest feature for you tosee is the hole the section plane passes thru on the right end of the front view.


You will get different environments and icons depending on the feature you are trying to edit. If you edit the sketch you will end up with an environment similar to the following:





Create or edit your sketch features and select the blue check to complete the feature.


If you edit the extrudethe followingdashboard will come up:





So to change the surface extrude to a solid one select your extrude feature in the model tree, select the right mouse button,select edit definition, and select the icon seen above. You should end up with something similar to this:





Here is the part with a section cut:





Looking at the sectioned solid can you see how the geometry isn't matching what is in the front view of the drawing. The large cylinder is the wrong type of geometry so remove that from the sketch. The inner rectangle leaves material you don't want so remove it. For the holes there is also material you don't want. The inner circle is the diameter of the thru hole and the outer circle is the diameter of the counterbore so remove the outer circle. Here is what you end up with by removing those features from the sketch:








From the drawing you want material along the bottom of the rectangle so remove that from the sketch. You'll end up with a block with two holes in it. See if you can get this far first.