Compound Line like in SolidWorks? 1

[SS65SuperNova]

Hi, I am new to ProE. I am using Wildfire 3.0. At work we just have the basic ProE licenses. I am trying to design hoses and exhaust tubing. I used to do so in SolidWorks when I needed a brake hose for example. I would sketch two sketches in different planes, then use the compound line feature to make it one projected sketch, then sweep one hose.

Is there anything in ProE that will let me do something similar?

Thanks

 

[seymours2571]

Yup...here is how to do it:

1) Change your filter from "smart" to "geometry"
2) LMB the first curve
3) Now press and hold the shift button (your highlighted red curve will no longer be highlighted).
4) With the shift button still pressed, LMB both the first curve and second curve (both should be highlighted red now)
5) Now click the copy button and then the past button (or ctrl c then ctrl v).
6) The drop down will now allow the curve to be either exact or approximate.
7) Click the green check box and presto! Compound curve.

In wildfire PTC changed the way these things were created. I think it is totally confusing. In the previous menu driven proe it was much easier to create these compound curves.

Hope this helps,

Steve

Stephen Seymour, PE
Seymour Engineering & Consulting Group

http://www.seymourecg.com

 

[SS65SuperNova]

Steve, I tried that, but all it did was copy the two lines still on different planes. It didn't combine them for me. What is "LMB"? I selected the line, maybe that is my problem?

 

[SS65SuperNova]

I figured it out! Simple...I just selected the two individual lines then went to the "edit" tab and selected "intersect".

But if you get around to it Steve, let me know what LMB is?

Thanks for the help.


Billy

 

[dgallup]

LMB = Left Mouse Button

 

[seymours2571]

The original lines will still be on two planes, however you will have to query select while in the sweep function. The new name of your compound line will be something like Copy_1. That is the feature you would need to select for your sweep path.

I tried the intersect method you spoke of but on the two curves I created it trimmed the other one. However, I didn't even know you could do that. Learned something new today.

Steve

Stephen Seymour, PE
Seymour Engineering & Consulting Group

http://www.seymourecg.com

 

[mjcole]

Stephen,

To add to the great (* worthy) information you've provided so far.

It all depends on the 2 profiles or sections (sketches) used
If a portion of sketch 1 or 2 doesn't intersect the other when projected, the two projection or compound curve cannot exist at that location.

In regard to ?MB, some people use LMB, MMB, RMB for Left Middle Right. Which reflects our societies point of view that people should be right handed whether they want to or not.

The PCC or (Personal Computerically Correct) way to refer to mouse buttons that I've used from time to time is MB1, MB2, MB3 in order of use so Lefties and Righties can understand what you mean no matter your own preference.

To prevent this from causing issues be sure to make the Max,Min extents of both curves so that you will end up with a complete curve and not have gaps. One nice thing about Pro/E is that if you have extra resultant curves that you don't need to use you can hide these on a Layer. The Pro/E Projected Curves can be created in more ways than the SolidWorks nonEquivalent. SolidWorks only gives Sketch on Sketch OR Sketch on Surface options whereas Pro/E can project any edge or curve on surface if needed without having to extract that item to a Sketch to make it work.

To figure out how to achieeve Features in Wildfire as you did in 2001 and earlier versions you can use the equivalent Menu Mapper where you select the menu items you used to and find out what the equivalent process is on Wildfire. I have disliked the Object Action only approach that PTC has implemented in the new interface. It may make more sense to users who don't have the entire Menu Manager interface burned into their memory like I and most likely you do.

Pro/E Menu Mapper link

Too bad it's 1 y 1 and they got rid of most of the Menu Manager on Right. All functions can still be found from drop downs.

Another Way to figure out how it's done is to Activate Legacy Mode [Applications > Legacy] create the feature then go back to Standard under Applications and redefine the feature.

I've kind of learned that if you want to do a surface merge you activate the Quilt selection manager or my "sq" Select Quilts mapkey. You'll notice that the Edit Feature > Trim, Intersect, Cut icons are not accessible unless you have 1 Quilt selected. Same thing is true about the pattern feature icon. At least with Wildfire you can create your own icons and Flyouts if they don't exist which is not possible on some other programs.

Michael