Centering sketch on grid

[RainMan52]

I'm not really an autodesk inventor novice (more intermidiate user), and have discovered a trick that Solid Edge (that we use at school) seem to have that i can't get to work in inventor.

 

in solid edge, you can center your sketch onto the main grid line, basically making the center of your sckeetch "0" on the X,Y,Z planes.

 

 

I tried doing the move command, but you can't snap the sketch to the grid. the snap to grid option down't work because one you start putting in dimentions, it doesn't constrain the origine of the grid to the center of your sketch (or the one tyou deifine)

 

 

has anyone here, more adavanced than me found a way to get this to work ?

 

 

thanks in advance.

[Aussiemike]

Rainman52, see if this is what your after,

 

1. Open standard part

2. Now your looking at the sketch grid

3. In the browser press the plus sign beside origin

4. Left click the centre point

5. Whilst its highlighted click on project geometry

6. You will now have a fixed dot from which to start you sketch from

7. Make sure the dot goes green when you start your sketch.

 

Cheers

Mike

[shift1313]

because there isnt really a 0,0 on the sketch plane is why you are having trouble. If you snap to the center of the grid for the first object you draw, you can place a grounded constraint on that and it wont move. If you constrain everything else to this you will get what you are aiming for. There is an edit coord system button but i honestly have never used it. I just use my constraints to drive the sketch and usually make one point on my drawing grounded and my "0,0" even though its not really.

[RainMan52]

Thanks alot guys.

I'll test it out when I get home.

[Aardvark]

Shift,

 

I would HIGHLY discourage suggesting that you use a fix constraint (or grounding for that matter) for any reason. The only exception would be to ground a SINGLE component in an assembly. The Origin planes,axis, and point are there for a reason. ALWAYS constrain your first sketch in a part to the origin point and when ever possible dimension and constrain to the origin features. This creates a much more robust, easily editable and functional model. Also when features change you will not loose constraints.

 

RainMan,

 

There is an option in tools/options that will automatically project the origin point on sketch creation. Look for posts by JDMather and follow the link in his signature for some very good tutorials.

[shift1313]

aardvark. placing a fixed constrain within a sketch shouldnt have any affect outside of the sketch right? I have used fixed before within a sketch within an assembly and have no issues moving or constraining components and i can go back and modify the sketch at any point. I wouldnt just use fix on anything, it has to be appropriate. i think you are speaking about grounding a component in an assembly correct? or have i said something wrong.

 

I must have misread the question, i thought he was talking about moving an entire drawing around in the sketch plane. Rainman, can you clear up what you are trying to do, i misunderstood.

[Aardvark]

Placing a fix constraint in a sketch has a huge effect outside of the sketch! If you fix a point and it is not attached logically to the origin then trying to use the origin for mirroring, patterning, extruding, etc is useless. The origin planes are the backbone of your design, they are inviolate and cannot be removed. If you use them to design your parts you will have healthier parts and assemblies.

 

If you have a spherical part that is not constrained to the origin how do you constrain it to anything else? Pretty much your only option is to use a tangent constrain which is a poor choice at best.

 

I can create an assembly made of parts logically designed about their origin axis that can be assembled constraining only to their origin axis that is impossible to break.

 

Fix is just a lazy way of fully constraining a sketch that will cause problems for you later.

 

Sorry for highjacking this thread.

 

Shift,

 

If we want to continue this discussion, lets start a new thread.

[RainMan52]

ok..here's my problem

youll find the info on the screenshots.

in solid edge (image name: SolidE1 up to SolidE3)

there is an option for this called "connect"

 

where you can connect the center of a line to any other element in the drawing space even the axis.

that way, you can center and constrain your geometry to the center of the axis in question.

 

My teacher just tought us this modeling procedure where when your geometry and part is centerd to all axis it's easier to Edit instead of creating a new plane each time you want to mirror something or edit something else that needs a referance.

 

 

I can't seem to find a similar option on Inventor

and I've been using it for about 6 moths now.

(imge name: My screen)

 

 

 

Look at the images and tell me what you think...hope it's less confusing now.

[RainMan52]

This is what I'm trying to achieve.

 

and please don't even ask me how I did it...it's so obvious and a bad way to work, that i don,t even want to discribe it....it would bring disonor to this board...

[Aardvark]

Did you read my first post? There is a check box in tools/options ( I cannot remember which tab but probably sketch) that will automatically project the origin point into new sketches. You can then constrain your sketch to the origin point.

 

Or you can do this manually by selecting the "project geometry" tool and selecting the origin points,axis, or planes from your model tree.

[shift1313]

aardvark, from there would you use a coincident constraint with the center point of the sides of the rectangle?

[Aardvark]

I would draw a construction line between the corners and constrain the origin to the midpoint of my construction line (Tip #21 on page 8 of this document;

http://home.pct.edu/~jmather/AU2007/MA105-1L%20Mather.pdf

have you read this yet? If not I would highly recommend it.).

[shift1313]

i will, just havent had the time yet.

[RainMan52]

I would draw a construction line between the corners and constrain the origin to the midpoint of my construction line (Tip #21 on page 8 of this document;

 

have you read this yet? If not I would highly recommend it.).

 

that,s exacly what I did in the inventor screenrint..

 

But I'm an architectual carpenter

so i rarely have a rectangle on my screen

 

and it losses all constraints to the center point once you start editing it...

[RainMan52]

Did you read my first post? There is a check box in tools/options ( I cannot remember which tab but probably sketch) that will automatically project the origin point into new sketches. You can then constrain your sketch to the origin point.

 

Or you can do this manually by selecting the "project geometry" tool and selecting the origin points,axis, or planes from your model tree.

 

 

you simply see the center point and can connect to it

but you don,t have any constraint to it, unless you do some geometric acrobatics with your sketch...

 

it

it's not really realistic in a production environement.

 

especially when you have to manually "write" G code fro a CNC

 

(yeah i know there are softwares out there) ...but try telling that to my boss after he has spend quite a lil forturne for Inventor and the upgrades...)

[Aardvark]

Projecting the geometry creates actual geometry that you can constrain to. Yes, it should auto-constrain if you have the geometry projected. In your screenshot I only see the grid lines (which are not geometry and cannot be constrained to. They will produce "soft" constraints which means that it will snap to the point but not attach with a constraint.). Furthermore, I don't see any construction lines in your screenshot. For examples of this and how it will react to different changes of the sketch see JD's document that I have posted several links to.

 

(JD if only you and I got royalties every time I mentioned that document....)

[shift1313]

make sure that button is on project geometry, there is also a drop down for project cutting edge i think and im not sure if that will produce the same thing.

[RainMan52]

sigh...I'll try to keep this on the low, but I'm starting to think my teacher was right when he told me "I told you so" on the subject that solid edge is better than Inventor when it comes to sketching and modeling...

I've been through JMather's guides with zoom at 150% and I must tell you, that you need to make quite allot of geometric acrobatics in order to have your cake and eat it too...where as solid edge gives it to you with just one click...

 

Don't get me wrong , I'm againts dumbing down things like Mac is doing right now, but over complicating it is the other extreem. Especially when you are talking about geometry...

 

This was my review.

 

And I still love Inventor over solid Edge because as a guy born in the mid 80's, sticked with one game consol brand from 93' tup untill 01' for another that I've stuck with till today, Studied computer management in College and deffends PC over Mac with violence, not even knowing what the hell mac has to offer, think that someonehow pepsi is better than coke...etc... etc...

to sum it up...i'm a fan boy.

 

 

thanx for the help guys

[RainMan52]

lol...my boss is going to be so pissed btw....he does the G code for the cnc....Hopefully we won't get a complicated order and he won't have to fire me

 

And yes s h i f t, I've used your technic.

only issue is that,

 

I have useless lines in my geometry that makes 3d editing look and feel like philosophy class...random and mind boggling.

 

if I remove those lines I lose the constraints

[Aardvark]

Each program has it's strengths and weaknesses. A lot of the time its more a matter of "it's not how (insert program name here) does it" than that one way is more complex than the other, you just have to get used to the way things are done and find the shortcuts (I assure you they are there if you want to find them). For instance if you don't want to go through all that trouble there are addins out there that will produce a midpoint located rectangle (I don't remember where though).

 

I just had to learn CATIA. Feel glad that Inventor and Solidedge are as similar in function as they are, CATIA will make you insane....