New sketch always centering on the origin point

[Anonymous]

Everytime I start a new sketch, I would like the screen to stay where it is on the part I am designing, but instead it always jumps away and zooms out centering on the origin point somewhere way off in the distance and then I have to zoom out to find the design and then zoom in on it and re-orientate myself. It wastes some much of my time!

Is there anyway of turning this off so the screen stays where it is when I start a new sketch please? It would make my life so much easier! Oh and for anyone who is about to post that I should sketch around the origin point, please don't, I don't like being around the point, I like to be away on a plane somewhere. (A bit like real life lol.)

Thanks 🙂

[Anonymous]

Hello Rob.

I didn't like being around the origin point either, when I started working in inventor. Occasionally I went as far as to delete the origin, just because I could. Eventually I realized that there is a reasoning behind it. Personally I abhore the entire idea of a sketch.

Regardless of my likes and dislikes, working away on a plane somewhere will most likely cause you severe issues with geometry later on, when you get into deriving parts from solids and using parameters. If you haven't locked down all dimensions in regard to not only each other but to the origin as well, as soon as you change the value of a dimension, it will break your design.

Specifically about why your new sketches jump around, there might be some settings that control that behaviour. I cannot remember to have ever fiddled with the manner in which new sketches open and mine do not jump away to focus on the point of origin.

It would be helpful to know which version of Inventor you are working in. Might make it easier for other people (more knowledgeable than me) to help you. Maybe you could also attach a part file as an example of said behaviour?

Hope you'll get some help.

BR,
Kami

[jmackniak]

right clicking on the dog house next to the view cube.  there you can set you view and your home view etc.  not sure if it will become a default setting.

[AdamAG99T]

I'm not sure if it is possible to both look at the plane while staying centered on the face/plane you're creating the sketch on, but it may be worth looking at these options. You can find the application options under the Tools tab on the ribbon.

[Anonymous]

Hi Maki,

Thanks for that response and you may have just inadvertantly answered
another problem I alwyas have of when I change certain dimensions, unless
everything is literally locked down, certain parts of the sketch jump all
over the place.

So my new questions are: firstly, how on Earth do you delete the origin!?
Bear in mind that I don't actually do full professional work so at most I
am only ever working on a single part, and then maybe an assembly but not
really - however, I may need to in the future soooo,

Secondly, how/where do I learn about locking sketches to the actual origin
so none of all of this crap happens ha ha!?

I am using inventor 2019.

Thanks.

[jmackniak]

to learn about locking sketches to the actual origin so none of all of this crap happens look into 'constraining' your sketches.   aka sketch constraints.  What you want to make sure is that your sketch lines are turning purple and not green.   When the entire sketch is constrained it will be all purple and on the bottom right corner of the user interface it should tell you that the sketch is fully constrained.  or tell you it is missing constraints.  

[jtylerbc]

---

@Anonymous wrote:
Thanks for that response and you may have just inadvertantly answered
another problem I alwyas have of when I change certain dimensions, unless
everything is literally locked down, certain parts of the sketch jump all
over the place.

---

That's to be expected when you aren't properly constraining your sketches, which usually involves attaching them to the origin in some manner (even if that "attachment" is actually dimensions locating the geometry at a distance away from the origin).  By refusing to use the origin correctly (or at all), you are essentially choosing to create unstable models.

---

@Anonymous wrote:
So my new questions are: firstly, how on Earth do you delete the origin!?

---

Technically you don't.  The actual origin is a read-only, 3D object.  It can't be deleted, moved, or edited in any way.  However, the origin point is projected into the sketch as a 2D point.  When talking about the "origin" in a 2D sketch, this projected copy is what people are generally referring to.  The projected copy is what you can actually delete, and doing so isn't any different than deleting any other sketch object, except for the fact that in most cases you should be using it instead of deleting it. 

If anything, it's too easy to delete, which is why "How do I get the origin back in my sketch after I deleted it by mistake?" is a common question for new users.

---

@Anonymous wrote:
Secondly, how/where do I learn about locking sketches to the actual origin
so none of all of this crap happens ha ha!?

---

It's been a long time since I've been through an Inventor training course as a student, so I'm not sure how they're organized these days.  But in the internal training course I wrote (and teach) for my company, this is covered before the first bathroom break.  I believe it should be included in some of the sketch and constraint-related tutorials that come with Inventor as well, though I haven't looked at those in a while either.  Sketch constraining, including the basic principle of referencing the origin, should be one of the first things a new Inventor user learns.

[Anonymous]

Hi jmackniak,

Yes thanks for that info. However, I know full well how to constrain my
sketches in relation to it's self, just no to the origin. I can make it all
go blue too but that's not always a good idea, nor is it always useful at
the start of a sketch...

thanks.

[Anonymous]

Hi jtylerbc,

Ok so we've established that locking some part of the sketch to the origin
by a dimension line at least, should stop all other parts of it jumping all
over the place as long as everything it constrained to that too. This is
obvious. Yes it's sketching 101 to constrain stuff, I've just never done it
to the origin before. I thoguht there may have been some different method
to do that. To be honest, it just seemed a little too obvious. I never
actually realised you have to link to the origin and thought you could just
make things wherever you wanted and they would behave lol. Apparently not.

However, that still doesn't answer the problem of why if I put a
freestnading circle in the middle my sketch somewhere because I don't quite
know where it will go or what size it is yet, when I then change the
dimension it jumps all the way over the other side of the sketch or
something. I can't constrain it yet because I don't know where exactly it's
going to go!? Or to be more accurate - I don't *want* to constrain it yet!
Any way around that?

In regards to the deletion of the origin. I understand what you mean. I can
delete the projectde one, I just thought he meant the original. As
supsected, you can't.

[AdamAG99T]

To fix the issue of the sketch jumping around when first placing a constraint go to the Application options and uncheck the Auto-scale sketch geometries on initial dimension option. 

[Anonymous]

Yes! I remember this! It definitely works for the most part. It still
sometimes does it but nowhere near as often thank you 🙂

[jtylerbc · Accepted solution]

Yeah, the option that @AdamAG99T should solve most of that.

That rescaling effect was added a few years ago as a solution to a different problem.  Before that, there was a tendency for sketched shapes to get distorted if they were drawn way smaller or way bigger than the real intended size, then a dimension was added.  What that function does is scale all the geometry in the sketch based on the first dimension added, in order to maintain the same shape and proportions.

This has some side effects in certain situations, which I'm not sure anyone really thought of before the change went live.  One of those is exactly what you're seeing - when you add a dimension to underconstrained geometry, the object moves because of the scaling.

Most users (in my experience) have a very strong opinion of this option.  They either love it, or they think it's the dumbest thing ever, and very little in between.  I'm firmly in the "love it" camp, personally, because one of my sketching habits has the side effect of preventing the scaling effect from moving the geometry.

I tend to geometrically constrain objects as much as possible (including attaching them to the origin however makes sense for the part) before adding any dimensions.  Essentially, I get the shape locked in before I worry about the size.  That scaled-movement thing isn't the original reason why I do that, but it has the happy side effect of preventing it.

[johnsonshiue]

Hi! I hope most of your questions have been answered by forum experts. One thing you may consider is to use Sketch Block workflow. This is one of the hidden secret in Inventor new users. In 2D Sketch environment, right-click on Ribbon -> check Layout panel. Now, you can easily create sketch block by selecting sketch geometry. The nice thing about sketch blocks is that they are rigid (unlike rubberband). And, you can insert multiple occurrences within the sketch and other sketches in the part. You can even derive them to a new part.

Many thanks!

[Anonymous]

Hi Rob,

unless I am really really wrong, it is not possible to fully constrain any geometry without linking it to the origin point with dimensions and/or geometric constraints.

The reason for this only becomes apparent when you work with multi-body part files, then derive solids as separate parts and then set up an assembly. If you link your initial multi-body part to the origin, then you will not have to set up any constraints in the assembly, all you need to do is to "ground and root component". This happens because all of your parts come from the same source part and thusly share the same point of origin.

And yes, I know what you mean about not liking the origin. When I began working in inventor a couple of years ago, I didn't quite like the restrictive manner in which some things are set up. But there is (mostly) a reason for all of it.

BR,

Kami

[Anonymous]

Hi Kami,

Ok thanks for this. The more people are saying the more I am realising that
actually, I don't need to worry so much because you all sound like you do
far more complicated work than I do! I literally only make single parts
with no need to make assemblies other than to see what it all looks like
stuck together lol. Don't even need to be able to function as they should.
So yeah, thanks though!

Rob.

[Anonymous]

Ok, interesting thanks. Not seen this before, I'll give it a look.

[Anonymous]

Hi jtylerbc,

That's the first full and accurate response I have had for that problem
thank you! I have actually posted about it before too. This original post
was simply about why the view always recentres on the origin everytime I
start a new sketch, and whether or not that can be turned off, but it went
on a slight tangent. I'm glad though because what you say is accurate and
makes sense and should help me develop better practice to avoid that now so
thanks! 🙂

[Anonymous]

Hi Rob,

If you are only going to be working with simple parts, I think you'd be better off using sketchup or blender or something along those lines. 🙂

Inventor is good at what it does but the question is, do you need what it can offer you? Then there's the question of pricing, is it worth using inventor making simple parts? Personally, I don't think so.

The point is, as much as I don't like it, Inventor is pretty good at doing what it is supposed to do (with some exceptions) but in order to do what it does, it is really restrictive. Sometimes you do things like you imagine them and then you find out that, even though the result is ok, you did not follow the workflow inbuilt in the program so the program will punish you later. I have been punished. And punished. And still am 😛

If you are using inventor just to model some simple parts, that's fine. But if in a year's time you think you might need to make more out of inventor, then investing time in doing things right is really worth it. And I mean WORTH it.

Personally, I only use inventor because the school makes me. But for creative work, you don't need all the specialized fluff in inventor. What I mean is this: I can design a perfectly good and functional looking table in sketchup in 10 minutes. Designing the very same object in inventor will take me twice that. The difference is that the sketchup table will only be a nice image, a concept design, while the inventor table can be refined until you have enough technical documentation to have the table produced halfways across the globe.

I apologize for perhaps sounding patronizing and all that. I am merely attempting to provide information I wish someone had given me before I began working with inventor. For the first six months, I kept trying to find ways to force inventor to do things they way I wanted it to do them, without realizing that I was fighting - and occasionally won - a battle while I had already lost the war. Once I let it go and went with the flow, inventor became a tool rather than an annoyance... as long as I do things the way it wants me to... 😛

Have fun 🙂

BR,
Kami

[Anonymous]

Hi Kami,

Well thanks for that lol. The thing is, my designs are complex in
themselves, I just meant I don't make more than just one part at a time and
they don't have lots of moving parts like a lot of other jobs I am hearing
about. It's perfect what I need, I just wanted to be able to star a new
skectch without the view centering on the origin point everytime lol.

But thanks anyway 😉

[Anonymous]

Hi Rob,

am glad that the users in here were able to help you.

As for the rest... Been there, done that, bought the t-shirt 😛 Meaning that I know what you mean. 🙂

Good luck, have fun and good weekend 🙂

BR,
Kami