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Moving datum in a sketch

10 REPLIES 10
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Message 1 of 11
safiredesignengineers
1411 Views, 10 Replies

Moving datum in a sketch

Hi group

 

in inv 2012, if I create a new part with adaptivity within an assembly the datum of the sketch ends up wherever, if I break links and remove the adaptivity, is it possible to move the absolute datum of the sketch to a decent position within the sketch?

 

Regards Adrian

10 REPLIES 10
Message 2 of 11

The world datum is fixed, you can edit sketch coordinates but I don't think this is what you're asking.

You would have to move the sketch profile to the datum rather than the datum to the sketch profile.

I maybe wrong and someone will probably correct me if I am.

The projected edges or points probably turn into grounded entities.

You may be able to show constraints and delete the ground lock constraint but I think if they are reference entities they are locked down completely.

Might be easier redrawing the profile where you want it and reselecting the feature with the new profile, don't delete the reference profile till you see everything works.

Watch out for assembly constraints going down the pan.

Move body might be another option but yuk, messy, and still doesn't move the sketch or the datum.

Message 3 of 11

Hi Harco

 

Thanks for your reply,  First of the goal: I want to move the sketch to datum or datum to sketch to tidy stuff up.

When making a part based on projected bits in an assembly it becomes a bit messy in the sketch and this can cause further issues later on in the design. I like to try and have a part evenly extruded and made around datum so the use of it's natural planes is better for constraining in assemblies.

 

You can break links and remove adaptivity which makes all projected lines un-constrained, these can then be reconstrained or deleted .

 

I can move the sketch after breaking links etc.. but I consider this slightly risky as with the sketch unconstrained it is possible to accidental move something! (it isn't possible to lock and group the shape in sketch and still move it)

 

I use other cad packages and they don't use constraints as they are not parametric modelers but if you grab the corner of a rectangle and move it - it moves, in inventor if you do this to an unconstrained rectangle it changes shape.

 

What would be good is if a sketch have a option to lock geometry so it can't change size or shape but allow it to move within the normal sketch environment and also have a group option so any features could be grouped to move together.

Then the whole sketch could be moved with less risk.

 

or to make life a lot easier, if the datum point could be moved to a chosen position then it would save a load of time and hassle!

 

regards Adrian

 

 

 

 

 

Message 4 of 11

You should be able to dimension and constrain your profile within itself and allow it to move without collapsing.

Then 2 constraints minimum to locate at datum.

 

If you can't manage this then window select the whole profile and use move to get it to the datum.

Message 5 of 11

Hi Harco

 

yes but that is a lot of work to constrain everything properly, see the enclosed 2d sketch, This had to have a new datum on it. the original sketch which I produced in a different package (because it has better 2d facilities for design development like this) was imported this as a dxf and then I created my 3d part. there is a lot of lines and arcs in a part like this, and it would take a while to constrain and auto constrain is messy.

 

I do use "window select" and this works and after I use the lock constraint to lock everything down prior to extrusion.

 

However I would like to not move the sketch if possible in it's unconstrained state as there is a chance of disturbing it! by moving the sketch datum the sketch will not need touching so little or no risk.

 

or if the sketch could be grouped so it could be moved as one object this would work, this could be a selection in the constraints?

Message 6 of 11

Hi safiredesignengineer,

 

 


the original sketch which I produced in a different package (because it has better 2d facilities for design development like this)

Having come from an AutoCAD background I understand what you're saying, and I know that sometimes there are layout tasks that as just much easier in AutoCAD (or some other 2D software), but in looking at the screen grab you provided, I think that part should take only a few minutes to model in Inventor (I see only 4 features, 2 patterns and a mirror feature). Here's a link that might help.

http://inventortrenches.blogspot.com/2011/03/inventor-101-simple-fully-constrained.html

 

 

Speaking to your original question though, I have had the need to paste in complex geometry from AutoCAD and have found that the best way to do so is to place it into a sketch Block (Creat Block button on the Layout panel of the Sketch tab), and then define the insert point. Then you can move and rotate all of that messy geometry as a single object.

 

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

 

 

Message 7 of 11

Yes, Curtis has taken the words out of my mouth, sketch block.

This will give you the grouping that you want, it will still be unconstrained in the block but if you never edit it then it shouldn't matter.

And again I agree about the patterns, but only as features not sketch patterns especially the tooth features, I would almost guarantee they would fail as a sketch pattern.

 

Listen to the man he knows what he's talking about.

Message 8 of 11

Hi Curtis and Harco

 

Thanks for your input.

Yes it is an easy item to model in inventor when you have the required known data, But this part along with some others needed to be "invented" and produced so that they would all work together in the required way.  Each tooth is built up of a few lines and arcs to get the clearance and tolerances required.

I did this in another 2d/3d package as it enables me to work very easily and quickly in a large workspace and on all the individual sketch designs together referencing off each other and various versions of the design as it progresses and develops.

 

This could all of be done in inventor no problem but time is money. I try to do as much as possible in inventor but sometimes it is best done in other packages and imported. I am sure many other users will do the same?

 

I could use sketch blocks but this still has the problem of unconstrained "flexible sketches" withing the block. The sketch needs locking down so it is not flexible but is still movable.

 

It would be good if at the import stage there was an option to import as a sketch block? so that the insert point could be set and the lock all constraint switched on. This would work.

 

I do think that the inventor sketch environment is lacking a load of facilities and tools that would really improve the product.

 

Regards Adrian

 

 

 

 

Message 9 of 11

Hi safiredesignengineer,

 

I suppose you could window select all of the line work, and then use a Fix constraint to nail down the geometry, then create the block. Or create the block, then edit it and use the Fix constraint.

 

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

 

 

Message 10 of 11

Hi Curtis

 

Thankyou for your input, I have been able to do this in a variouse ways no problem although using sketch blocks is a good idea.

But as per the origonal question it would be so much easier and safer if we could change the Datum postion to the sketch.

8-)

 

regards Adrian

Message 11 of 11

To answer your original query, the way I do it is to create the new part within the assembly, come back out of sketch and part edit, then constrain the part geometry to whatever you want it to referenced to. You then go back into the part and sketch edit and your sketch datum is in the correct position before you start projecting or drawing anything.

 

In general within a sketch you can move everything on the sketch at once using the move command, but I wouldn't use it normally because you risk losing constraints.

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