Radial Tubes and trimming

[Anonymous]

Hi Inventor Experts,

I would like to know if my request is possible in Inventor?

I have a Pipe header (30 inches OD)

and some Radial Tube connections to the header. 

I have named and constrained construction lines radially to the header.

I did a sweep for the radial tubes but I don't want them to the center but an offset point internally to the header (1/4" inside penetration).

Please see the attached snapshot if this can visualize my request.

The radial angle has to be parametric, in other words, I am creating a template as much as possible. please give some ideas about how can I accomplish this request, Thanks

[JDMather]

Looks easy to me.

Attach your file(s) here and end all doubt.

[Anonymous]

JDMather,

Please see the attached zip file and let me know if that will help to understand my request. Thanks in advance.

[Anonymous]

JDMather, 

Just to let you know that I tried the split command but I cannot delete the internal section.

Also, all the construction lines need to stay because if something is modified, everything will be updated.

Any suggestions are welcome. Regards

[johnsonshiue]

Hi! I took a quick look. I think it should be doable if I understood the request correctly. You can simply use Extrude -> Cut -> and select one of the circular profiles -> Through All.

Does it work for you?

Many thanks!

[Anonymous]

Hi JD, I just tried your suggestion, I think you meant Sweep, Cut, but for this option, it doesn't accept the bends. Or in the other hand, Extrude, Cut, it doesn't work with bends either. I used the split option instead but it also cut the sketch line for the parameter Ang_rqd= 30 deg, since this is needed for any changes in the parameter. Maybe I'm doing too much in sketches, it should be like the pipe engagement to a fitting. Like in SW or threaded fittings. I still looking for a solution. But thanks for taking the time to look in this matter. I'm pretty sure that you can come up with another one. Regards, Sam

[Anonymous · Accepted solution]

Sam,

I see a number of problems with your model.  You are not fully constrained and you are using 3D sketches.  Your pendant tubes' axes are all in the same plane, so sketch them on your XY plane and constrain to the origin.  Fully constrained sketches are all black lines, i.e no green lines. Purple lines are projected lines and are constrained by their very nature.  I would redraw using your parameters, but instead terminate your sketched pendant paths at the location where you want them to terminate.  There is no need to extend the pendant center lines to the header center point, you can make the lines coincident to the header center point.  Once you have that sketch sorted you can make a plane centered between your two sketched headers and perpendicular to the pendant's sketched paths.  On that plane you can project your sketched pendant paths and sketch your tube profiles from those centers. You  can then use those two sketches to sweep each tube individually.

[Anonymous]

SBean,

Thank you so much for your time in this matter. I think that is the best solution. I am going to try it. If you don't mind can you sent me your working file, for comparison and in case I am missing something? The reason I have 3D sketches was the idea to make part of the whole Assembly, but after looking at your suggestion I realize that it was the right way I should start it. I just have about a month learning Inventor. So I am looking for quick training by myself, but sometimes there is nothing close for I am looking so I posted for help and Here it is, Thanks to you so much.

[Anonymous]

Hi sbean, I am working in your solution, but I have a problem to make the lines constrain to the center of the circle. I drew a line from the center then I placed the angle, I trimmed the line at the required point, but if I change the angle the center of the angle becomes the breaking point. Can you show me what steps I am missing? Thanks

[Anonymous · Accepted solution]

I can tell you are new and learning, so i took it easy on you.  I have attached the file.  I would recommend changing the parameters from "Model Parameters to"User Parameters" by going to manage tab and selecting the parameter button.  Create user parameters at the bottom (you will have to change the name of the model parameters before creating the user parameters, and then re-dimension using new user parameters).  It will make it easier on you if you decide to go to a spreadsheet driven model.  Since it looks like you are going to make an assembly of your parts, I made the attached a multi body part that then can be turned into individual parts and an assembly.  Research multi body parts.

[Anonymous]

Thank you so much sbean, after a little understanding I found that the constraint was perpendicular to the circle, and It worked out, but your input is much beyond my appreciation to understand my future intentions, you have read my mind. Excellent!

[Anonymous]

Mr. sbean, You have saved it in version 2019 right I am working in Inventor 2018. can you save it in version 2018 as well? Thank you

[Anonymous · Accepted solution]

Sorry, but it would require a rebuild in an earlier version for you to see how it was built.  I suggest installing a newer version.

[Anonymous]

sbean, No Problem, Thank you, Anyway I got the idea and it seems to be working. I have more option that I need to incorporate on it, so I am in baby steps, like you already notice I am looking for some kind of template parametric iLogic modeling. I will post it later for your input to improve it if you don't mind. Regards, Sam