How to align two circles? (newbie)

[CNSZU]

Hello,

Assume we have two circles, one to the left and one to the right. What is the way to constrain the center points horizontally to each other?

I've tried selecting the circles and only get the constraint options "fixed", "fully fixed", "concentric", "perpendicular", "tangent" and "equal radius". But where is the constraint for "horizontal"?

The only way I can make it work is to create a horizontal line, convert it to reference, select the left circle and the line, choose "point on curve", then select the right circle and the line and choose "point on curve". That is a lot of work to align two circles! Isn't there an easier way?

 

[JohnRBaker]

You've already found the answer.

But you seem perplexed. Let me ask you, what aspect of a circle could possibly imply the concept of 'horizontal'? And then when you introduce a second circle into the 'equation' how does one imply that they are aligned? Again, what aspect of a circle implies 'alignment'? There is nothing. The line IS the answer since it can be BOTH 'horizontal' (a characteristic that is easy to comprehend when dealing with a line) and you can take the one aspect of the circle which is needed in this situation, it's center, and constrain it (for both circles) to the line, hence 'aligning' them. As I said, it's the Line that provided the needed characteristics AND which allowed you to create the desired relationship BETWEEN the two circles.

Anyway, I hope you understand that often one needs additional items to accomplish what you're looking for. Otherwise it's like trying to solve for 3 unknowns with only 2 equations.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

To an Engineer, the glass is twice as big as it needs to be.

 

[CNSZU]

My apologies for not providing adequate context. I've been using Solidworks, which is renowned for it's speed and efficiency. With that software, you can sketch two circles, select both of their center points, and then in the context sensitive popup menu select "Make Horizontal". This will align the center points of the circles horizontally. No need for additional sketching. It's fast and intuitive. I hope this makes sense.

Anyway, I was hoping for something similar in NX, and after realizing Catia also lacks this function, I guess I can't complain too much. However, the ability to sketch fast and inhibited is very important to me, so I'm trying to find every way to speed up the sketching and modeling process in NX.

 

[RAGudorf]

Switching from Solid Edge, which has this function as well, has defintely slowed the sketching process down of contraining hole centers. Especially when you have a lot of holes that cannot be patterned. In Edge, same thing. If the holes are less than 45deg off horizontal X direction, they will both constrain horizontal. If greater than 45, they will constrain Vertical. All with the same command. Very quick and painless.

--
Ryan Gudorf
CAD/CAM Supervisor
Budde Sheet Metal Works, Inc.
305 Leo St.
Dayton, Ohio, U.S.A. 45404
Tel: 937.224.0868
Fax: 937.224.1356

http://www.buddesheetmetal.com

 

[cowski]

Sounds like a nice option to have. For situations like this, you can contact GTAC (Siemens' technical team) and have them open what is called an 'Enhancement Request' (ER). This will alert the development team of features that the customers want/need in NX.

http://www.nxjournaling.com

 

[DaSalo]

NX requires no additional effort to accomplish the same thing. You simply need to do reverse the operation sequence. When you create a sketch in NX you can automatically allow it to pick a horizontal direction or you can define the horizontal manually. So lets say that you allow it to define the horizontal automatically. Once the sketch is launched you:

1) Create a line using the "Profile" tool. This tool launches automatically and the "Horizontal" constraint is created automatically (if you have not turned that function off). So creating the "relationship" part of this task is accomplished in exactly two mouse clicks; one for each end of the line.

2) Now click on the circle tool (If you have set up your radial popup menus this can be accomplished by holding down two buttons on you keyboard or SpaceExplorer and moving the mouse about .125 on the screen = very fast.) Place a circle on each endpoint of the line. This requires two mouse clicks per circle. The coincident constraint to the line endpoints should be created automatically if you have not changed the setting.

3) If you have autodimension turned on and you typed in the exact line length and circle diameters at the moment of creation you are all done. Auto dimensions will have been created for everything and your sketch will be fully constrained.

4) If you need the line to truly be a reference line you can right click it and turn it to reference from the flyout menu. There is usually no need to do this as almost any tool that uses sketch curves for geometry creation will allow you to select only the parts of the sketch you want to use.

So this task can be completed in 6 mouse clicks and the number of keyboard strokes required to type in the necessary dimensions. I would guess that this is exactly the same or, maybe, one mouse click more, than what would be required in Solidworks. It all depends on how you want to count the clicks required to open the context sensitive menu and then pull down to select the Horizontal constraint.

Solidworks and NX look alike in many ways but the fundamental thought process behind certain workflows is different. NX is much more flexible and there are many ways to accomplish very similar functions. You pay for this flexibility with a longer learning curve. It all depends on exactly what you are doing. If you aren't doing something that requires all of the power and flexibility that NX has under the hood you might not feel the benefits.

NX 7.5.4, NX 8.0.1.5
Tecnomatix Quality 8.0.1.3
PC-DMIS 2011 MR1

 

[Walterke]

Alternatively, you can draw a line from the center of one hole (make sure the option the snap to center holes is enabled) to the other center hole and constrain that line horizontal. It's a bit faster then using the 'point on curve' option.

You're just not used to thinking the way NX thinks (which is a bit different from solid edge).
As said before, you can do everything equally fast, just in a different way.
Practice makes perfect.

NX 7.5
Teamcenter 8

 

[CNSZU]

Walterke, the method you mentioned is actually more time consuming, assuming the circles are not drawn aligned to begin with, necessitating constraining the line afterwards. This will require in all 14 mouse clicks.

DaSalo, no doubt NX has more power than SW, but ironically in this case, wouldn't you agree that the SW sketcher with this particular constraint option is one step ahead? Let's count the mouse clicks:

NX
1 select line tool
2 click start of line
3 click end of line
4 mb2 (cancel line tool)
5 mb3 on line
6 select convert to reference (otherwise when creating eg extrusion we need to select option "region boundary curves" which takes even more time)
7 select circle tool
8 click line start point
9 click to complete circle
10 click line end point
11 click to complete circle

Solidworks
1 select circle tool
2 click to start circle
3 click to complete circle
4 click to start circle
5 click to complete circle
6 press esc to cancel circle tool
7 click center point of circle 1
8 ctrl click center point of circle 2
9 click "horizontal" on the properties page

In conclusion, for a simple sketch task of creating 2 horizontally aligned circles, SW is 18% faster than NX.

 

[JohnRBaker]

I can't take credit for thinking of this as someone else pointed me to this approach.

If you're only interested in having the two circle in your sketch positionally aligned in a 'horizontal' manner then try this workflow:

Create your first circle wherever you wish.

While still in the circle creation mode place your cursor (don't push any mouse buttons, just hold it there) over the center of the first circle until you see the center point highlight.

Now move the cursor to either the Left or the Right (without pushing any mouse buttons) and you will see a dotted line being 'rubberbaned' as you move the cursor.

As long as you see the dotted line you are maintaining a 'horizontal' alignment.

When you get to where you would like the second circle to be placed, simply push MB1 (Mouse Button ONE) and then drag the cursor until you have the circle size that you desire and then press MB1 a second time.

Note that this will also work to positionally align circles in a 'vertical' manner only instead of moving the cusor 'Left' or 'Right', you move it 'Up' or 'Down'.



John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

To an Engineer, the glass is twice as big as it needs to be.

 

[DaSalo]

----
1 select line tool
2 click start of line
3 click end of line
4 mb2 (cancel line tool)
5 mb3 on line
6 select convert to reference (otherwise when creating eg extrusion we need to select option "region boundary curves" which takes even more time)
7 select circle tool
8 click line start point
9 click to complete circle
10 click line end point
11 click to complete circle
----

You don't need to do step 1, it launches automatically when entering the sketch.

You don't need to do step 3, no need to specifically cancel a tool, just click on the next tool.

That gets us down to 9, which is identical to SW. My point isn't necessarily that NX is faster, just that it is not necessarily slower once you get comfortable with it and get your menus setup in an efficient way. You glossed over the radial pop-up menu option, which is a HUGE time saver for frequently used commands.

I'm also not saying that I wouldn't want to have the Solidworks functionality as another option. Sure I would. I'm sure I would use it at times. I don't feel like I'm suffering without it though. I also worked on Solidworks for several years before moving to NX. NX was more difficult and slower for me at first and it took me longer to learn than Solidworks. Now that I know it it is just as fast.

NX 7.5.4, NX 8.0.1.5
Tecnomatix Quality 8.0.1.3
PC-DMIS 2011 MR1

 

[CNSZU]

JohnRBaker, the method you described is simply "snapping" the circles into horizontal alignment as they are placed, it does not create a parametric horizontal constraint to ensure that they will always stay horizontal.

DaSalo, step 1 is needed because you're not always creating the line first thing the sketch starts. Sometimes you will draw it after drawing other elements, like arcs.

Step 3 again is needed, because you need to cancel the line tool in order to right click the line to convert it to reference (tested). However, let's try a different method, instead of right clicking to select convert to reference, we click the convert to reference tool directly:

1 select line tool
2 click start of line
3 click end of line
4 select "convert to reference" tool
5 select the line
6 mb2 to ok and close the tool.
7 select circle tool
8 click line start point
9 click to complete circle
10 click line end point
11 click to complete circle

It still comes to 11 clicks. However, I do agree with you on the radial popups, which I'm now investigating. They really seem to be well thought out, and definitely have potential to create geometry even faster than Solidworks. The brilliant thing is that you don't have just one popup, but three for the modeling application and three more for the sketching application. This way you can cram all common tools into radial popups and completely ignore the menu and toolbars, thus playing it like a piano.

Something a little off topic, I wish someone could arrange a live CAD speed competition, where the contestants are given a drawing with dimensions and constraints and are tasked with completing the model in the shortest amount of time using their preferred software and settings. Some of the CAD vendors will probably be willing to sponsor this competition. It will provide entertainment for us geeks as well as giving an indication of which software is the most time-efficient.

 

[JohnRBaker]

JohnRBaker, the method you described is simply "snapping" the circles into horizontal alignment as they are placed, it does not create a parametric horizontal constraint to ensure that they will always stay horizontal.

I NEVER said that it did. I was very careful in how I worded my reply, which leads me back to my original response to you and the fact that the 'cost' of creating an additional line is a small price to pay, as other have commented to that same effect in this thread.

Professional observation: Somehow equating the number of button clicks to the overall efficency and/or productivity of a piece of software is at best a fleeting concept. It's like back in the 80's when I was still working in sales and people used to bring stopwatches to a benchmark. It was true then and it's still true today; it's productivity and NOT performance which pays the bills, and while one may use a stopwatch (or the number of button pushes) to measure 'performance', it takes a calendar to measure 'productivity'. And for the record, I'll stake the productivity of NX and the Siemens PLM integrated family of products any day of the week...

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

To an Engineer, the glass is twice as big as it needs to be.

 

[man2007]

Well, there is another method to create the aligned circles. Create a horizontal line (make it reference if u want), and on Snap Point toolbar, switch on only 'point on curve' option. Now you can create as many aligned cirlcles as u can by selcting point on curve option for circle centre.