Snap to the centre of an open pipe end. How!!!!!!!???

[pendlej]

Why does fusion make it so hair pullingly difficult to snap to the centre of then end of pipe I have made. (see pic)

What good is only being able to snap to the edge if I need to line the centre of the pipe up with the centre of an outlet port.

Please can someone help.

[herzinj]

Hi Pendlej,

When I want to do something like this quickly, I usually just choose to create a sketch on that surface (or create a work plane there and create a sketch on it) and then choose to project the geometry of the circle.  It will give you a little dot at the center of the circle that you can snap to.  Of course, you could always just draw a line across the center of the circle as well and you will be able to snap to that midpoint.  Creating this sketch might be an extra step, but at least it only takes a few seconds!  Maybe someone else can add a better option here, but this should be a quick work around if nothing else.

James

[Anonymous]

Hi, maybe I can give you a few ideas here. I am a user of the program, not an expert or its software developer. There are a few ways but I will suggest two ways here.

a) Using "Align":

Without forming components from bodies (works on components as well)

1)  Use the "Construct" menu and select  "Point at center of circle/torus/sphere". This way you can just click construct menu, and select the "Point...."  then click the end of the pipe and the other opening, you will form two points at the center of both pipe and the other opening.

2) Select "Align" at the modify menu and click both ends. They will be aligned:

b) The second way is Using  "Joints" from the "Assemble" Menu:

First right click on the main bar of the browser, select to make components from bodies.

This only works on components. If you only have two bodies you will form two separate components.

Select the "Assemble" menu, select "Joint" and click both ends. They will join together.

Hope this will help you out. It is not that hard. Fusion 360 is already one of the easiest program to use for designers.

[Oceanconcepts]

I think what you are looking for (and I have been as well) is the ability to use the move tool to select the two centers and move one to the other.  That’s part of what is being asked for in this, one of the most voted ideas in the Idea Station:

 http://forums.autodesk.com/t5/fusion-360-ideastation-request-a/object-snap-is-really-needed/idi-p/38...

But the Align tool now works well in this context, and will allow you to snap centers. It is no longer necessary to create construction geometry to snap the centers together- it was in earlier versions, but the Fusion developers listen to requests.  

The example below is a solid in Model workspace. For a surface as in your example yo would select the outside edge of the end, and it will snap them concentric. 

Select the Align tool:

Select the point on the part you want to move

Select the point you want that to snap to

And it shall be done as you specify ;-). 

[pendlej]

Thanks for your replies but neither the align tool or the joint tool will let me select the centre of that pipe opening. On the photo if you can see that little line which I guess is the seam of the pipe, that's the only point of the circle end it will let me pick up, which is useless for what I need to do 😞

Also when I try and make a centre point through circle in the construct menu, it wont let me select the pipe.
This software is so frustrating at time. Simple things made extremely difficult at every turn.

[Anonymous]

Actually to make you feel good about using Fusion 360 the Fusion team should help you. Learning to use programs like this is sometimes very frustrating but once you get used to it it will be like magic. Well why not check your Select option and make sure that they are all selected. And also check your workspace. See what workspace you are currently using. See the attached screen shot. The Select Through option is very important:

Sorry I cannot help you anymore. The above is the last step I can ask you to check. In fact I know why you could not do what you intended to do but I would prefer to have a Fusion Team member to help you this time.

Have fun using the program! We all went throught that by the way!

[Anonymous]

Hi Ron, yes this new "Align" update does not require  "construction mid point" even with objects like hollow pipe. This user here had been trying to find the center point of his model that is why I showed him how to construct a point. I suspect his "Select" options are not fully checked.

Actually this new Align tools is close to the Snapping Tools that a lot of users had been requesting including I myself. It is quite useful. Another good tool after "Joint". Their new Creasing Capabilities are also wonderful.

Well Fusion 360 had become so big and powerful now I think lots of new members could be a little bit confused about DM Mode, Parametric Mode, Sculpt, etc.. Well so as other matured programs. All the 3D programs in the opened market are definitely not easy to use.. Both of us are lucky to had been following the Fusion Team development since the Beta days. I would say this user has a point that the Fusion Team should really look into. "How to keep new users interested in the program when they were frustrated?"

[joel.palioca]

Hello,

Are you able to attach your model here?  You can do this by going to the File dropdown and choosing export.  From there make sure the file format is archive.  You can either upload to the file here or email me at my email directly.  If you try to upload the file here and have an error you can try to rename the .f3d file as a .zip and it should upload correctly.

This way we can help resolve your issue directly with the model you have.  I have tried a number of different ways to create a pipe and all of them allow me to select the center of the pipe so I want to make sure that I haven't missed something specific to the way your creating your pipe.

Cheers,

[Oceanconcepts]

Kingson is right, all CAD tools have a learning curve. Like learning a new musical instrument, it's often the basics that are hardest at first. 

Is what I show in this screencast not what you are able to do? 

[Anonymous]

Hi Pendlej, you had posted a great question. You had made us rediscovering the new capabilities of the "Align" tool. Most of the users check this forum everyday because this is the place we can discover new tricks and tips from the users and the Fusion support team. Great work! I gave you a great Kudo on this!

[pendlej]

HI All,

Straight pipes created in the model section are fine and will pick up from the centre. Its the ends of pipes created in the sculpt window that just wont pick up. I checked selections and they are all enabled. My fix mentined above by creating a small solid disc in the centre of bothe ends worked as it allowed me to use the joint tool rather than the align tool. Align is great but once I had the pipe aligned into the outlet socket, it would always come out in the wrong rotation.

The fusion team need to add the ability to program in the angle of the align function, much like the joint function where it can rotate on its snap point.

A massive thanks to you all for your efforst and help. I am overwhelmed by the level of support and community spirit on here. Top notch.

One thing Fusion or even a third party need to do is make a training course for this program so that people like me can go on these courses and learn the correct way to do things. They have courses for inventor so why not fusion? Or even a comprehensive Fusion360 for dummies style textbook.

[Anonymous]

Hi there, I am glad that you are not frustrated anymore. Yes Fusion has evolved into something big and powerful, just as I had mentioned before. I saw that they had improved the way the tutorial is showing up in a Browser inside the Fusion windows. Now the program is available to the Mac App store download I would assume they will stay at the present desktop arrangement a bit longer. It had been changed many times during just the last 12 months but all to the good then the bad (??? some might not agree!). The parametric function is still not perfect but lots had already been changed. The "Create Form" and the "Create Base Feature" part is kind of non parametric but at time I had found that I could create my projects in the parametric mode but at the end I will save an archive parametric f3d to my local drive, then i will stop recording and work on Direct Modeling mode. I could do more things in that mode, for example you can shape a face of a model just by using the "Move Command". You will find that your problem might be solved for the time being by cancelling recording. I had to because of my line of designs that required a lot of scaling (for exmaple my ring designs for our shop, and pendant designs all need to be scaled to different sizes). Well Enjoy... Why not try the Direct Modeling mode, it might work better for you for the time being. Then you can go back to Parametric mode. I think Ron will agree on that too!

Greetings from Hong Kong

Kingson

[pendlej]

joel.palioca here is the attached archive file with the problem pipe. Please let me know your thoughts

[pendlej]

Oh believe me I'm still frustrated ;-). My workaround of the issue takes so much time its counter-productive. The program does lack a bit of 'common sense' at times. But I think if there were some training courses run for the program this would solve a lot of peoples issues with it.

You mention to stick to the model area instead of sculpt. This would be great but how would I create a pipe with a bend in it in the model window?

[Anonymous]

Sorry for so many Edit, but read my conclusion.

Hi there I also uploaded your f3d to my Fusion and I had found something and I attempted to fix for you. The Fusion Team might have other ideas but this is what I had found.

1) Your tube is an opened Patch type surface, not really a solid that can be selected. Screen Shot 1, body (30) is showing that it is a patch type surface.

 

To do that, I had created a solid cylinder with a hole in between called Body (32) in  Screen shot 1 to show you the joint action. I had dimmed out your other components.

Now you have to give your pipe Body 30 some kind of thickness to become a real solid. So you go to "Patch" workspace (Parametric Mode fine here) select your Body (30) and select Thicken. For example, I thickened that by 2.00 mm.  Screen Shot 2

You will see my Body 32 right next to your pipe, now a solid with a wall thickness of 2mm.

Now you switch back to "Model" workspace by selecting that at the browser window. Now you should be at the Model Workspace and you can see clearly Body32, the one I had created, and a new solid Body33, the one you had added a thickness of 2.00mm to surface patch body30. You can dim out the light bulb of body30  now. but do not delete that. Not at the parametric mode.

You cannot use "Align" here because it will not work on your pipe due to one reason or another. But Body 32, the one I created can. So to joint them together you have to use Joint at the Assembly menu.

To do that you have to create components from bodies. You select that at the browser top bar. Then you had created two new components: Component 37 and component 38.

The pipe (now a component) could not use Construct to get a mid point for some reason, so you have to use "Joint Origin" to create a joint origin and move that to the approximate middle of your pipe. There are ways to get the mid point of your pipe but that is another technique that you have to find out yourself. Not the scope of this simple demonstration. The Cylinder I created does not require that because it is perfectly round.

Now Click Joint and select both of your pipes (yours and mine) and they will joint together the way you wanted it:

By looking into your browser component structure, you had done a very good job. Maybe you should start creating some main components and sub components and move the related components into Sub-Assemblies. And provide better labeling to them.

I think your pipe creation must be done in a manner that resulted in a pipe that construct could not locate a mid point, nor "Align" can locate a point of reference at your pipe for the align works.

Anyway my demonstration seems a bit complicated but as a simple user that I am (definitely not an expert!), if I could fix that, you can too..... Well I had a lot of fun analyzing your model and believe me or not, I am not a member of the Fusion Team. Just a simple user.

My last Conclusion of your file: EASIEST IS TO DELETE BODY30, and use PIPE from the model workspace to create the pipe, select "Hollow" and give it some thickness. That will work with "Align"

My demonstration above just shows that if Body30 is created but the Sketch line deleted, then you have to do it that way. I found that your sketch line is still here. So Delete Body30, and use Model Workspace, Pipe to create a good round pipe!

Hope it helps you out. Have fun!

Cheer! from Hong Kong again.

[Anonymous]

Hi you might be right, we might not be able to use "Align" tool to align pipes formed in the "Create Form" or "Sculpt" workspace. Maybe a few updates later it can do that. For now, it is better to create those models that you planned to snap together at the model workspace at the "Create Base Feature"  parametric mode. Then you can always "Align" or join them together using "Joint".  If you want to align or Join pipes created at the Sculpt workspace, you might have to use "Joint Origin" to create a joint origin, then joint both pipes together.

[joel.palioca · Accepted solution]

Hello,

Alright so parsing through the past few posts it looks like there have been a few questions that have come out, let me see if I can help answer some of these.

Issues:

1. Unable to snap to the edge with pipe that originates from a T-Spline body.  This is shown in the model you have sent me.

2. How to create a pipe with a bend in it from the model window

3. Align doesn't have the ability to define an angle

1&2. Unable to snap to the center with pipe that originates from a T-Spline body.  This is shown in the model you have sent me.

As mentioned above the model that you sent me has a pipe that is referred to as Body30.  Looking at your time line, this body was created by leveraging a sketch with a couple straight lines, an arc acting as the bend in the pipe, and using that as the path for a T-Spline pipe body.  After that you exited the Sculpt workspace and the t-spline body was converted into what looks to be a surface.  The problem you have now is that you are unable to snap to the center of the pipe.  So there are two ways to approach this, we can either leverage the existing work you have done or we can create a new pipe.  If you are looking to do a lot of pipes and are expecting to do a lot of aligns, then I would recommend we create a new pipe.

It looks like you are leveraging a parametric model so we will try to keep with that.  One way to create a pipe is by using the sweep command instead of the pipe command.  I have a feeling that the reason you used a t-spline pipe is because in parametric models we don't have the pipe command in the model environment, though it does exist in direct modeling.  If you use the same path that you did with the t-spline body and create another sketch at the end of path with the profile you are looking to use, you will be able to create the same pipe, but it will be parametric and it will have the center point that you are looking for.  See the video below for an example with your model.

The other option would be to use a BaseFeature instead of the Form so that you can leverage the pipe command there.  After you create your pipe you will have to exit the BaseFeature so you keep your parametrics.  The downside to this right now is that you won't have any parametric control of your pipe, also if you need to create multiple pipes this may cause additional work.

If you wish to leverage the existing pipe that you have already created, you can use the Plane along Path command, and then offset another plane to the end of the geometry.  With the work plane created you should be able to project the geometry and then create a center point there that you can create a joint origin from.  This is something you may have already tried, and it can create some extra work.

3. For the issue to define an angle when you align, I will bring this up with the team and see what we can figure out for the future, right now the only control we are able to provide is the ability to flip.  For now though if you use one of the above workflows to make sure you have a center point to align, you should be able to leverage the move command from that same center point and use the rotate there.  I understand it is an extra step, but it may be a workaround for now.

Overall it sounds like you have also gotten a lot of good advice from some other users, hopefully this can help as well.

Please let me know if you have any other questions,

[Anonymous]

Hi Joel, thanks for this post. The Pipe created at the Sculpt (Create Form) workspace is not very accurate anyway. The two ends seems to be extended beyond the original Sketch curve. Is this a bug or that was the intension of this command? The pipe command in the Create Base Feature workspace seems to match up with the sketch curve. To create a projection from the converted TSpline Pipe to an offset plane created by Plane alone path seems to require some body splitting to match up the two ends of the curve. Then using project cut edges to get the center point.

Is it possible to have a little tip box from somewhere perhaps in the next few updates to alert the user that Pipes should be created at the DM mode if Center points are needed for other purposes like Joints or Alignment? or an option to switch to DM mode to create such pipe? That will save a lot of frustration from users.

Thanks for listening.

[Oceanconcepts]

Yes, this thread brings out several things that are potentially very frustrating for new users, and are a direct result of Fusion’s rapid evolution and unique approach to the design process- the things that make it great are also potential stumbling blocks. 

Getting the distinction between direct modeling and history/ parametric mode and understanding all the down the road differences in what you can do in each environment is hard to explain. It's like a neighborhood that has few street signs because it’s still being built. I find myself mostly in direct modeling, except when I’m exploring options that would benefit from being able to alter sketch lines and have things update. That’s mostly because the kinds of free form puzzle solving that I need to do result in ridiculous history timelines when I move a particular element 17 times trying to fit it all together. But if I place all the hard edged things where I need them in a Direct environment, I can use parametrics to tweak design details of my enclosures in a very efficient way. 

The distinction between “Sculpt”, which I think of as similar to working with clay, and the “Model” or “Patch” environment- more like working with machinery- is at the core of practical Fusion use. What sorts of parts make sense to create in each workspace? It’s more than what sort of shape, it’s what you want to do with the forms down the line.  

Maybe tutorials on the line of “If you want to do _____ then ____ is a good workflow”.  Things that address overall strategy would be helpful.

[Anonymous]

Hi Ron. I agree 1000% on your point of view. I too have to use direct modeling because of the needs to scale components.