Help me take charge of my sketches (rather than them take charge of me!)

[Anonymous]

I'm having some 'trouble shooting' Issues that I've been trying to figure out since I started using inventor not so long ago:

Projections
Using sketch projections is very useful, but one thing that I can't figure out is how to delete unused projected lines.

In the image attached, I only need to use part of the projection I created from my sliced model, but it seems that creating a projection from cut geometry was my only option. For the sake of a tiny line, I have a silhouette of my whole armchair, creating sketch geometry that is not only of no use, but I cannot delete it. They seem to be permanently fixed to the sketch.

Sketches included in view

When pressing Home or any of the other projections on the view cube, The model zooms out to fit the screen, and includes any of the visible sketches... including the centre points of any [large] radii. Why does this happen? For me at least, this feature is of no use, and is rather irritating.

Visibility

Is it possible to change the default visibility settings? For the most part, when completing a sketch I usually don't want to see the dimensions. It slows me down having to turn visibility of everything off every each time I do a sketch.

Sketch Items don't highlight in browser

This issue is actually happening to both sketches and parts; when I highlight a part or sketch in my graphics window, it doesn't highlight in the browser. This means If I want to find a part, i have to hover my mouse over the features in the browser until I find it; a pain if my features aren't all named, or I have a large feature tree.

Thanks in advance for your support.

[JDMather]

Attach Inventor file here.

[Anonymous]

No problem, file attahced.

[JDMather · Accepted solution]

There are enough issues here to keep me busy for a week - and I don't have that much time, so I'll cover just a few.

For projected geometry that you don't need, I would window select and change to Construction.

There is a way to delete unneeded projected geometry - but at your experience level - I think that would just get you into trouble.

You can redefine Home view by right clicking on the view cube.

 It is a simple right click Hide Dimensions.  If you don't want to see dimensions in an active sketch - then convert to a Sketch Block.

Shift right mouse to change selection priority filters.

Your Frame Profile sketch is not perpendicular to your Frame Sweep Path - resulting in an asymmetric model from the foundation.  No amount of editing after the fact will fix this.

I know your primary question was about sketching, and yes there are several issues there, but I have to get some of my own work done.  If someone else doesn't pick up this thread - I will try to come back to it in a couple of days.

I would have expected a beginner to start with the easier internals of the assembly, but I guess you do need a basic form to get started.  The old chicken and egg conundrum...

[Anonymous]

Hi JD,

Thanks for your message.

I've now converted the lines to construction, which I did do initially but was hoping there was a way delete them. This will have to do for now.

Thanks, i'll use the sketch blocks.

Well actually the profile and sweep path are perpendicular - The model orientation was actually changed  (via view cube), and thus the back is meant to angle downwards. (I realised about half way through that I over complicated things. Lesson learned).

It's fine, I totally appreciate that, and please don't priorities me at all! I'm getting stuck in learning the software, so after posting questions I usually just move on to learning some other element in the meantime. There's really no rush, contributors can chip in as and when/if they choose 🙂

"I would have expected a beginner to start with the easier internals of the assembly, but I guess you do need a basic form to get started.  The old chicken and egg conundrum..."

- I totally understand where you're coming from, and actually would agree ordinarily. However, as my objective is to both produce a model for manufacturing purposes and also to manipulate it to make it softer for rendering, I wanted to go the the process, get a foundation of my work flow, and then build on that.

Thanks for your time and input.

[JDMather]

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@Anonymous wrote:

Well actually the profile and sweep path are perpendicular -

Well actually no, they are not.

[todd_cannon · Accepted solution]

Hi lukefromharris,

I would be willing to bet that the reason you can't delete your projections is that you have a projected loop. Look in the browser where the sketch is and if it has a + sign next to it, expand it and see if a projected loop shows up. If so, you can right click it there and delete it. When projecting, be careful not to select a face if all you need is and edge. I usually make them construction at this point too. If you only project the edges that you need, they will delete like any other geometry. Hope this helps you understand projection.

Cheers,

Todd

[Anonymous]

Hi Todd,

Thanks for your feedback. Under the + it has 'projected cut' but it still does as you said, so thank you. As suggested, I converted what remained to construction geometry.

[Anonymous]

Hi JD,

Thanks for taking the time to make the video, it was very helpful. i apologise, I kept looking at the sketch thinking "i'm sure that's perpendicular??", but I understand completely now!

The issue began when initially modelling this feature. I had planned (and in fact attempted) to produce it with a loft; hence the mirrored, unused profile. I couldn't seem to get the profiles to loft, with the path as the guide curve. In a second attempt, I tried to copy and paste the profile to the YZ plane, but matching the form and constraints doesn't seem like a particularly easy task. In the end, I went with the sweep, and stupidly thought the problem would be taken care of when I created the extruded cut that with give m armchair its desired lean. Obviously this was completely ignorant to the fact my solid was asymmetrical! I also thought perhaps I could create some kind of end constraint that dictated the behaviour of my profile at both ends, but there didn't seem to be an option for that either.

[JDMather]

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@Anonymous wrote:

I couldn't seem to get the profiles to loft, 

In the end, I went with the sweep, 

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First step is to decide which of these two feature types will return the geometry that matches your Design Intent.

Once that decision is made - we can get either one of these two techniques to work (properly).

If you are not sure - it might be a good idea to create two parallel files - each one using a different approach.

[Anonymous]

Hi JD,

Thanks, great idea. I took the opportunity to explore sketch blocks, and with the aid of this I managed to solve the modelling issue; rolling back, I rebuilt it as a loft with the first profile saved as one block and the mirrored profile saved as the other. And shazam! I always wondered how one would create a loft using profiles that are similar/the same, as copying and pasting removed all of the constraints. I wish I had discovered it before.

Now I just need to solve the highlight issue with my browser. Though perhaps this is a software bug?

[JDMather]

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@Anonymous wrote:

Now I just need to solve the highlight issue with my browser. Though perhaps this is a software bug?

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Click on sketch entity.

Right click>Find in Browser.

[Anonymous]

Hi JD,

Thanks for your input, but that doesn't help me unfortunately. The issue happens with parts to. When hovering my mouse over the part/feature, it doesn't highlight in the browser.

[JDMather · Accepted solution]

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@Anonymous wrote:

 When hovering my mouse over the part/feature, it doesn't highlight in the browser.

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Parts are very different things than features.

Find in Browser works for Parts.

For Features - simply click on the feature....

[Anonymous]

I understand. Thanks I got it!

[lena.talkhina]

Hello @Anonymous  !

Great to see you here on Inventor Forum.

Did you find a solution?
If yes, please click on the "Accept as Solution" button as then also other community users can easily find and benefit from the information.
If not please don't hesitate to give an update here in your topic so all members know what ́s the progression on your question is and what might be helpful to achieve what you ́re looking for. 🙂

[Anonymous]

Hey Lena,

Thanks for your message. I did, partly, and also several of the replies answered different parts of my question. Whats the best approach here? I want to avoid selecting one answer, as it may not help other look for answer to my other questions.

[lena.talkhina]

Hey there!

Thanks for coming back to the thread. You can mark more than one comment as accepted solution - I think it's a best way in this case.

But, don't hesitate to continue discussion here, you never now how it will go out, right!

Glad to see you again and let me know if you need any community assistance 🙂

[Anonymous]

Oh great, I didn't know that! I learn something knew every time 🙂

Thanks for your support.