How do I snap to references in sketcher?

[SvenW]

I've used Wildfire 2.0 previously, so I asked to get Proe installed in my new job. I got Wildfire 4.0 and all is well and fine, except that the handy feature of the sketcher snapping automatically to references is missing or inactive, and for the life of me I can't seem to figure out how to activate it. What I'd like to do specifically is tie the centerpoints of lines to references, but no amount of dragging around the middle points makes them to adhere to references... not finding any useful information from ProE help or google (with keywords 'snap', 'snap to feature' and 'snap to reference'), I'm starting to pull my hair out which certainly isn't helping the cause.

I did find one seemingly similar call for help in this forum, but the thread was ended by the originator telling he already found another thread addressing the problem and had solved it, but there was no link to this thread, or any solution. I'd be very thankfull of any suggestions.

-Sven

 

[m-d-e]

Go to sketch mode, press Sketch --> Options --> Constraints tab. Check the constraints you want the sketcher to assume.

That's how it's done in WF5. Hope it helps.

Edited by: m-d-e

 

[SvenW]

I have checked this tab, and all options are checked. These constraints are also automatically applied, midpoints just dont snap to references.

As a matter of fact, the constraints seem to behave a bit differently compared to 2.0, for example when connecting two circles with a line, it doesn't seem to suggest double tangency...

 

[jraquet]

In WF4:


While in sketcher mode, select the menu item Sketch > References.


If you need to pick the center of an edge, make sure you reference the edge and not the surface. To try it out make a square extrusion. For the second feature or sketch the default references will be the two datums normal to the sketch view.


Select Sketch > References and roll over the top edge. You'll note that the reference is shown as Surf: F*(EXTRUDE_#). If you right click to roll through the options, the next reference shown should be Edge: F*(EXTRUDE_#).


(where F* is the feature number and EXTRUDE_# feature type ?).


With an edge selected/referenced the reference is limited by the length of the edge and you can find a midpoint or an edpoint.

 

[jraquet]

If you are going to pick new referenced or add references frequently in sketcher it is a pain to Sketch > References. You can add the referenced option to your sketch toolbar.


While in sketch mode, go to Tools > Customize Screen...


Under the Commands tab, select the Sketch categories there is an icon for references


View attachment 4683


You can drag the references tool to the sketch toolbar:


View attachment 4684


I think it should be a default icon but...


Hope that helps

 

[SvenW]

Thanks Jeff, those are all good tips. Unfortunately not quite what I was looking for, though. I'll give an example of what I'm trying to do:

I'm at the sketcher window, with the two standard reference planes. I wan't to make a centered square, so I click once somewhere in the upper left hand quadrant of the screen, and then click again somewhere in the lower right hand quadrant so that the square is approximately centered. Then I choose the point tool, and add midpoints to two edges of the square. As I have purposefully drawn the square approximately in the middle, I want the the midpoints to automatically attach to the reference lines. But this doesn't happen, and no amount of dragging the midpoint around will attach them. So even if I add midpoints, I still have to give four dimensions, and changing one will force me to change the one other dimension too, if I rescale the square. This will not do.

I don't remember ever having to configure this behaviout on Wildfire 2, it was just there. It wasn't there with Wildfire 4, but I refuse to believe that such a useful feature would have been removed.

 

[doronron1]

Try adding centrelines to the reference planes first, then draw your box.

 

[zpaolo]

I worked with WF 2.0 and I am now on WF 5.0, but as far as I remember it has always worked like this: if you draw the square as you said and then add a point, this point can snap to the middle of the square edge OR to the reference line. You can place it on the middle with the automatic snap, then add a constraint to snap it on the reference line. Was it different in WF 2.0?

Paolo

 

[jraquet]

Place centerlinesand use symmetry rather than midpoints.


If you place the centerlines on the vertical and horizontal datums and then start your square in the upper left quadrant, as you drag your mouse to place the square it will snap to symmetry when the distance is approximately the same on the other side of the centerline.

 

[Ceeeeez]

Best response to your problem:

You're stuck! They've removed the ability to do what you're asking. I noticed the same thing when I went from Wildfire 2 to 3. They have not given back this auto-midpoint snap in Wildfire 4 or 5... it's just GONE. So you can stop pulling you hair out.

Everyone else's response is... "do more work to make it act like it used to act automatically". Yet NO ONE sees a problem with this. I don't WANT to spend more time adding points, aligning them, making them symmetric, adding center lines... BLAH. What happened to "LESS MOUSE CLICKS"?

PTC simply removed this feature and no one complained so... its gone.

 

[krow72]

SvenW - you can use constraints to get what you want. After you have the midpoints created go to constraints and use "create same points" (see attached pic) then pic the midpoint and then the ref line. The point and line should move to the ref line.


View attachment 5348


View attachment 5349


View attachment 5350

 

[garymig]

Sven, A more simple aproach, I use a grid with snap on. Perfect centered square.


It works every time.


Gary

 

[SvenW]

Best response to your problem:

You're stuck! They've removed the ability to do what you're asking. I noticed the same thing when I went from Wildfire 2 to 3. They have not given back this auto-midpoint snap in Wildfire 4 or 5... it's just GONE. So you can stop pulling you hair out.

Everyone else's response is... "do more work to make it act like it used to act automatically". Yet NO ONE sees a problem with this. I don't WANT to spend more time adding points, aligning them, making them symmetric, adding center lines... BLAH. What happened to "LESS MOUSE CLICKS"?

PTC simply removed this feature and no one complained so... its gone.

Thanks for the new replies, although this thread is a bit old . I've switched jobs since and regrettably don't use Pro/E at the moment, but I hope others find the clues helpful.


It seems that the quoted text pretty much nailed it; you can achieve the same effect, but it's way more work than it used to be, and for me this is a problem. In an environmentthat expectscomplete constraints making my models symmetric comes to me naturally, and Pro/E of old supported me in this. I seriously do not understand why such a usefull and value adding feat has been removed. It's about eliminating the unnecessary mouse clicks, and in this case this objective has failed miserably.


I did find workarounds when this was still current for me, but I was after a real fix and now it seemsone isnot to be found.


I actually went to PTC's website today, hoping to find an email address for customer feedback. Didn't find one, though I'll admit i didn'twaste all that much company time on this curiosity. Anyway, stuff like thatought tobe very easy to find... I guess they're not that interested.