Solidworks gurus

[D-man]

OK Guys, can any of you tell me how i would create a blank to fit to the end of this 160mm pvc pipe? blank must go with all coutures.

im looking to blank that area off with 5mm pvc sheet then plastic weld into place either inside the pipe or on the cut edge.

image here > Screenshot by Lightshot (http://prntscr.com/1mikw3)

Part is attached for more information

Anyone gurus out there feel brave enough to teach me how to do it?

[mekanik]

Hi D-man
Is the aim of the exercise to just blank the bore of the fitting ?
If so depends on the pressure it is going to see, but you could make a expanding bung. it's just two circular disc's bolt welded in centre of one and a clearance hole in the other with a doughnut shaped soft sponge rubber ring between the two, tightening the two plates expands the rubber and locks the assembly in the bore. Plump Centre stock this sort of thing.

[D-man]

Hi D-man
Is the aim of the exercise to just blank the bore of the fitting ?
If so depends on the pressure it is going to see, but you could make a expanding bung. it's just two circular disc's bolt welded in centre of one and a clearance hole in the other with a doughnut shaped soft sponge rubber ring between the two, tightening the two plates expands the rubber and locks the assembly in the bore. Plump Centre stock this sort of thing.

Thanks, I know of these bungs as I'm a filtration engineers and pipe fitter by trade.

The aim of the exercise is to ask the gurus of solidworks, how they would go about designing a 5mm PVC sheet and contour it to the cut area. I will Try get an image up of what I mean.

The reason for this cut in the pipe is to enable that pipe and the other half to sit lower in a bowl shaped component. Then it will be pulled with concrete half way up the pipe.

[D-man]

Ok this is what I'm looking to do. I need to learn how to make the bit that's pointed out. So it fits nicely against the cut part, with a little overhang all round for a bead of plastic welding. :-)
http://img.tapatalk.com/d/13/08/21/4e4ajaqa.jpg

[mekanik]

No problem- cardboard template, it's that simple

[D-man]

Yeah, but I need to be able to draw it in solidworks so I can send the drawings to the client for them to approve buddy.

I understand the cardboard and then scan, redraw etc but then to get the fold in also. I just don't know.

[mekanik]

My bad i just thought it was a job you wanted doing and did not require approval from someone else, i know a man who has on the forum but he would tell you to make a template cut the plastic weld it and stop ******* about. sorry i can't help.
Regards
Mike

[JAZZCNC]

D-Man,

Send me just the pipe has the assembly won't show them because the individual components are missing. . . Or send all individual components.!!

[D-man]

Cheers Dean, Email sent.

[Danielroyal25]

Hi d man,

I know it's plastic your after not sheet metal, but it may benefit you to draw it via sheet metal features as it will give you the option to obtain the flat pattern if needed.
If you sketch a oversized square the click base flange/tab and apply thickness and guage table (solidworks standard one) then create a sketch (single line) horizontally across the square and click sketch bend you can the fold the piece to suit the angle on your pipe. If you then insert this into your assembly and mate it fully you can then look normal to the pipe. Edit the new part in place and create a new sketch on the correct plane. Create an offset from the outer diameter of the pipe to give you the weld surface and then complete an extrude cut (with normal to selected) through all cutting the outer portion of the new part away. This should leave you with your desired part. Hope this makes sense.

[D-man]

Thanks I tried that and got close but maybe I missed something out as I just can't do it lol

[JAZZCNC]

Thanks I tried that and got close but maybe I missed something out as I just can't do it lol

D. . . I can do it no problem but trying to explain so you can repeat is the hard part.!! . . .There's a few ways but this is easiest I think to explain.

This way is pretty much the same as Dan's just different.!! .. Lol

First start a new part.
Create a sketch on front plane to use has a reference sketch. With the dimensions like in pic1

Then from sheet metal select Base Flange/Tab and select front plane. Using convert entity select the rectangle from reference sketch.
Click Ok and the select the thickness etc you want.

Next select Sketch bend, select the rear face of the Base flange you created. Then using convert entity select the bed line and click ok.
Now click above the line to create fixed face, Now select outside bend position then enter 68.93deg in angle box.
Click Ok and hey presto it's bent.

Next select extruded cut and select face on Top piece of bend. Then using convert entity select circle and click ok.
Now in direction 1 choose through all and select flip side to cut. Click side 2 then click ok and Hey presto there's your part which can be flattened if needed.

Hope this makes sense.

[D-man]

Ahhh I will give it another go!

Jazz that file I sent you earlier may not work because I've just opened it on my laptop and I'm a couple bits missing lol but I'm making headway with solidworks

[JAZZCNC]

Ahhh I will give it another go!

Jazz that file I sent you earlier may not work because I've just opened it on my laptop and I'm a couple bits missing lol but I'm making headway with solidworks

Yes I've just looked and only screws show. . LOL . . . .It's because it's an assembly and you didn't include the components.
I opened in viewer so can see it and will look closer but in mean time if you create another then send me the components.

[D-man]

Haha oops!

[D-man]

New file sent lol

[vargai]

removed xxxx