struggling with basic tiny stuff.. what are these ? and why is that ? inventor

[Anonymous]

Hii ,

I had redo the whole H frame, mattress and plank underneath using extrusion method suggested by Curtis (except for the H frame, i used 2 sketches and 2 extrusion method = still consider as 1 solid instead of 2 ).. and all good , but this is not the issue here.

 i did those 3 solid directly in a brand new assembly file. after sketch, extrusion and i constrained them.

this is just to show you what i have done.

then i faced a few confusion and i have one question as well.

during the assembly of the mattress and the plank, i asked myself one question:

1st question, is there no constraint that will constrains MID POINT of the Mattress to MID POINT of the Plank under it ?  i mean it is so simple in real life, just grab and put it there and adjust a bit.. there it go. although the 2 objects are not of same length, but it is easy to stack them mid to mid.

and not to mention doing that in autocad 2d is also super easy with MID POINT SNAP feature..

is there no such "advance" feature in inventor ?

since there is no such feature in inventor, hence i have to use the constrain to one side with an offset value method.  which let me think that inventor still has got room for improvement in these basic stuff.

this pic below just to show you that now that i have done doing and assemble the 3 solids.

then i clicked "create"

and now my confusion comes!

"select sketch plane for base feature" what does that mean ?

because latter on when i click "new 2dsketch" button, and

IT WILL ask me to "select plane to create sketch or an existing sketch to edit"

my confusion is what's the different between 1st select sketch and 2nd select plane ?

can someone explain to me what is the 1st one different then the 2nd selection of plane/ sketch ? because as i selected it, i didn't see much different.. or rather to say i didn't see the point of 1st time selection of sketch ..

what can or cannot  i select or shld i select for the first selection request ?

the 2nd selection is so that we can adhere our new sketch to the selection that we just made, else, user mind found out later that the part is not created 90 degree to the plane it intended,  am i right ?

1st request for selection of sketch , i think i clicked on one of the plane of the origin of the  assembly file. but i don't know what effect has it..

here shows photo of me clicked the "2dsketch" button.. to create a 2d sketch.

it asked me for selection 2 time. then what's the 1 selection for ?

because my goal now is to create a staircase cabinet leaning against the H frame, hence i chose to select H surface as sketch selection.

there you go, selected H frame as base plane of the staircase cabinet sketch plane.

take a look, this center point at the bottom left corner is exactly where i started with when i was doing H frame..

btw, is Center point (of the browser) is = ORIGIN of 0,0,0 of the sketch ?

 however when i zoomed in, and find out that the "center point" of both the assembly file and my Highbedframe is not as same as the location where i left it off.. 

which should be at the left corner of the foot of the highbedframe....

this kind of thing caused me "not confident" toward selecting a starting point of line when i am doing a line.

who know? such a minor false selection of point (thinking it is the corner of the highbedframe) will ended me out with lot of troubleshooting of measurement and correction at later part of the designing project (if i only manage to find the fault after everything else is done designing). 

ok, move on... this is where i will start my laddercabinet.

appreciate your time and patient for helping me.

thank you.

andrew

[asiteur]

That's A LOT in one post but I will try to answer them all.

1) You could contrain mids using a Joint, which is the new type of constraining in Inventor. If you use a rigid joint and select the midplanes then they will be fixed at once. Having said that, I rarely use it.

2)select sketch plane for base feature"  Basically, when you create a part in place this lets you define your reference. If you have a ramp at a certain slope and you click that as sketch plane your X,Y,Z in the part will be relative to that. Differently put, it allows you to have a coordinate system other than the one in the assembly.

OK to be honest I lost you after this. I hope this helps already.

[mcgyvr]

If you modeled properly using the "Born technique" then to align the middle of the mattress to the middle of the bed frame you simply constrain the origin planes..

See attached model showing how the origin planes were used to center the mattress in the frame

As to your 1st sketch plane.. When you create a part in the context of an assembly it needs a "face" to create your first sketch on.. Its asking you to select that..

After that you are in the context of the part and then it wants a part plane or other face to sketch on..

Then I lost patience and didnt' read any further.. 🙂

[mcgyvr]

and here is some reading on the "Born" method..

see attached..

[jtylerbc]

@Anonymous,you seem to be having trouble getting out of the AutoCAD mindset.  I see this a lot at my company, since we use both programs (for different purposes), and used to be almost exclusively AutoCAD.  Hopefully I can help steer you toward the way you need to approach things in Inventor, which is very different from AutoCAD.

1. You don't need a separate constraint type to constrain the "mid" of one object to the "mid" of another.  You use the same Mate and Flush constraints you've been using elsewhere, but you apply them to the origin planes of the parts instead of faces (assuming you modeled the part around the origin, which you generally should be doing).  In the case where you have a good reason to not me modeled around the origin, you can create a midplane to constrain to using Work Planes.  Lines (and part edges) have midpoints, 3D parts don't.  Constraining to the midpoints of edges is possible, but usually isn't what you want (constraining to a point essentially creates a ball joint).

2. When creating a component in-place in an assembly, the message "select sketch plane for base feature" means exactly what it says.  You are selecting the plane on an existing object (another part face, an assembly origin plane, etc.) that you want the first sketch of your new part to be located on.  You also have the option (via a checkbox) to automatically constrain the part at that plane.  This first selection is creating a sketch, but it is creating it in such a way that it also defines the initial location of your new part in the assembly.  Until you understand the way this works, you may be better off creating most of your parts individually, then dropping them into the assembly and constraining them into place.  One thing you need to get out of your mind is the AutoCAD-based idea that you are making "solids".  You're not - you're making parts.  In Inventor, the term "Solid" is used to describe the individual bodies in a part that contains multiple bodies.  There is no such thing as a "solid" in an assembly.

Your post is rather long, so I may have missed some things in there, but I think this hits the major points of what you are asking about.  Most of the rest of your post seems to be more specific cases of these two issues and their effects.  If something is still unclear, post back with your additional questions.

[cbenner]

@Anonymous

Hi,... you're basically asking for an entire tutorial here.  May I suggest breaking your post up into individual questions?  Not many people are going to have the time to tackle this entire thing.

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@Anonymous wrote:

Hii ,

during the assembly of the mattress and the plank, i asked myself one question:

1st question, is there no constraint that will constrains MID POINT of the Mattress to MID POINT of the Plank under it ?  i mean it is so simple in real life, just grab and put it there and adjust a bit.. there it go. although the 2 objects are not of same length, but it is easy to stack them mid to mid.

and not to mention doing that in autocad 2d is also super easy with MID POINT SNAP feature..

is there no such "advance" feature in inventor ?

thank you.

andrew

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In this question, can you use origin planes to accomplish this?  Or add work planes that will accomplish this?  What exactly do you mean by mid point?  Do you mean mid plane?  Or the 3D center point of the mattress? 

[Ray_Feiler]

I think you should consider going through the built in tutorials first.

[Anonymous]

Hii,

Thank you for the joint feature.. it is super good. thank you.

i have tried your 1st point.. it works beautifully..

but the 2nd point of yours.. i still couldn't get the confusion cleared.

if a video of it will most likely able to help better.

tq