Future move tool enhancements?

[O.Tan]

Hi,

I'm not sure where to post this up, here or IdeaStation. But here goes:

So, I end up with this situation, the hole you're seeing right now is created in bodies, so when I convert to component, it seem that I can't move that hole. Problem is, that hole already has some joints in it and no matter what I do, it seem the only way to reposition is to delete and redo the joint again.

I've tried creating a hole (as you see in the vid), and I notice that repositioning only allows me to snap it onto points, there's no way for me to reposition the hole using some form of cartesian system.

This is my suggestions:
1. Make a tool that'll convert these dumb features into smart features (this will have the added benefit that F360 will be able to read imported models and add some intelligence to it; here's an example: https://www.youtube.com/watch?v=ARvSUH41ick. If I recall correctly, besides recognizing holes, SolidEdge is now able to recognize fillets, and chamfers) 
2. Improve the move tool by adding another object option "features" to be able to move features like hole, fillets and chamfers. 

Extra: Recognizing holes will be a huge benefit as simple round features can now be converted to a hole feature and gain extra features. 

Thanks

 https://screencast.autodesk.com/Embed/7d8c8449-0739-4c44-98a5-19c877606802

[O.Tan]

Odd that I'm unable to embed screencast. This is the error it gives me after I copy pasted and previewed the embed code in HTML:

[carl_bass]

This doesn't answer your real request (I'll let the development team do that) but it might help in the short term. Instead of trying to move the hole, select the hole and choose edit. That should allow you to reposition it

[O.Tan]

Sadly the hole isn't a hole but a circle that's cut thru. So I'm unable to move it like how a normal hole feature would 🙂

[karyeka · Accepted solution]

Hi O.Tan,

Can you try following things?

1. Regarding "there's no way for me to reposition the hole using some form of cartesian system"

I use the references (side edges of the face I am creating hole) in the hole dialog, to position the center of the hole with exact values. 

Pls refer to the video - https://screencast.autodesk.com/main/details/a92ba64d-203b-4dfd-96fe-420275c2fb04

2. Regarding "recognize holes"

We have Find Features tool that detects holes among other things on a body. However, it's only available in Direct Modeling envrionment right now. It's not part of Parametric or Timeline/History toolset yet. 

Please refer to the video - https://screencast.autodesk.com/main/details/4d604334-295e-43d0-bf58-dc3633266f15

where I converted the document into Direct Modeling document and used Find Features to detect hole on an imported step model. After I find Hole I can edit it with right mouse on the Hole feature in the browser. However in this workflow when we convert to Direct Modeling document we loose timeline and history and that may not be desirable at all. 

When I import a step model it comes in as Base Feature. Ideally I would just edit the Base Feature to get into Direct Modeling toolset. However, I noticed that when I run Find Features in this workflow the browser doesn't update to show the Hole feature (even though it seems to have find it). This is a bug and we will work on fixing it. Please check this workflow at - https://screencast.autodesk.com/main/details/264d8712-f5bb-46e1-90a3-41ad95fbabd0

3. Regarding "improve Move to move features like holes"

Again, we have Move Faces just in Direct Modeling environment as of now. I typically select hole face and move it to move the hole. Please check the video at - https://screencast.autodesk.com/main/details/57cc1d54-40d7-411f-b1de-53b21c5cc833

Let us know if this helps or if I have misunderstood anything. I will work with Product Management for your requests/ideas.

Thanks,

Anand

Fusion360 Development

[O.Tan]

1. Aaah, so that's what reference is for, embarassing how I didn't manage to figure it out. Now that you show me (thanks), the implementation is quite intuitive. 

2. Yup, finally found it. I remember seeing it somewhere , but I never managed to get it to work cause it's a habit of mine to:

• Draw a round hole in sketch
• Extrude the sketch

Because of this, Fusion registers the hole as an extrude feature, so using the find feature will result in no hole to be found, what I recently learned to do is that I first need to dissolve the extrude feature and only run the Find Features tool, then it'll work like how it should.

3. Got it, I didn't realize that just like in SolidEdge, some features in DM and HM is slightly different and some isn't available. 

Thanks for the thorough reply karyeka!

[Oceanconcepts]

Just to throw a few more Fusion thoughts out there which might be helpful to you with holes or any other feature:  I have found that Fusion is spectacularly capable- in direct modeling- when you just select all the surfaces you want to move and use the Move tool- granted, this is relative motion, and you don't have the ability to position precisely with reference to other geometry unless you measure or place construction features, but you can reorient the manipulator.  When you want to move a cutout portion or a feature 5 mm in a specific direction, this can often be a very easy path. Particularly for those, like me, who don't plan ahead very carefully. 

re. the screencast posting, this is very unclear in the forum interface- it seems as if you should be able to place it as a video- that's what the button says. What you need to do is to go to the html tab in the edit post window, and paste the embed code into the HTML text outside any <p> tags.  At least that's what has worked for me. 

[O.Tan]

Yeah, it's quite capable in direct modelling mode and I do use it when I work in a larger assembly as the timeline history will just be too long. Until F360 Supports 3D Object Snapping, we will have to live with measuring to where we want to move the geometry 

[karyeka]

Fusion 360 supports object snapping, you don't have to measure distances before moving geometry. In the Move command we have "pont to point" transform type. As you select that and hover over analytical faces the software gives you potential snap points either to specify distance to move or align bodies/components to others. The snap points are available for Brep analytic faces, T-Splines, sketch and even grid points. 

Please check out the screencast - https://screencast.autodesk.com/main/details/c164ebe3-284c-48b2-9cb0-2448c336b3e2

Is this what you were looking for?

Thanks,

Anand

Fusion360 Development

[O.Tan]

Oh wow, how did I not know of such features! This is what I'm looking for, thanks!

Edit: still need some more time to get used to it, once I'm use with it, I'll probably report back if I encounter any form of "limitations" with it

[karyeka]

sure, thanks. Looking forward to getting feedback.

Thanks,

Anand

Fusion360 Development

[O.Tan]

Hmm, odd behaviour here, can't seem to lengthen the slot made via the slot tool. 

https://screencast.autodesk.com/main/details/75da9960-6a01-4bb1-8a4c-5c89caa7f6ab

[karyeka]

Indeed odd. It seems to move all the tangent connected faces together. I tried with some non-tangent faces and it works, as shown below in the video. However, I understand that's not the intent here.

I will update as we debug more.

In the meantime workaround (for Direct modeling env) is to extrude the 2 side faces a bit and then select new vent faces and the round face to move (lengthen) the slot. The 2 side faces can then be pulled back. It's not elegant but works. 

(In the parameteric env you can always change the slot length)

https://screencast.autodesk.com/main/details/7b4a7991-80ce-4215-96e6-06dbf0d7c0fe

Thanks,

Anand

Fusion360 Development