Making a simple plate cap (part) for a 12.75" OD pipe. I've tried with projections, section cuts, curves, skewed planes, etc to make a part with the elliptical shape but always run into some problem such as a sketch that won't project on the skewed plane but reverts back to a perpendicular plane. Or "items can not be converted" or something.
This seems like it would be childishly simple, but it is killing me.
See attached, I only want to make caps for the ends that fit the skewed cut.
Hi Mike
You can you just draw an ellipse yourself?
Something like this ?
note the equal relation is on the selected lines and the driven dimension is grey not black
Could you upload your file.
Maha Nadarasa wrote:
Could you upload your file.
Do you collect them :-D
B.R.
After seeing the file only I have to decide whether I have to collect it or not.
Yes, the file is easy to assess, worse with women. Even after thorough knowledge, after marriage they sometimes turn out to be devils ;-)
Hello,
I'm assuming these end plates are welded onto the pipe.
If this is true, then you will need to:
If #1, then create a sketch on the 45° end of the pipe.
Convert entities on he ID & OD and change these ellipses to construction.
Create a construction line from the major apex of the ID to the major of the OD.
Do the same at the minor apex.
Create an ellipse with the major snapped to the midpoint of the major construction line and the minor snapped to the midpoint of the minor line.
This sizes the end plate at mid wall thickness. (You can opt to use fixed major & minor distances from the OD, too so set the weld bead size.)
Extrude the end plate to the required thickness and uncheck merge.
Mirror the end plate about the middle of the pipe (use body option)
By setting the edge of the end plate back from the pipe OD, your end plate can be cut normal to its face.
If the end plate edge is flush to the OD, then the perimeter, in addition to added a weld chamfer, will need to have a sinusoidal, non-normal cut (which, I'm certain will be a more expensive operation).
Kevin
Am I missing something? Weldment End Caps?
Brian Graves wrote:
Am I missing something? Weldment End Caps?
This is not always reasonable. When creating drawings, it can create a problem (BOM, the welded structure appears in the assembly as one part). This cap you can do it without Weldmet.
B. R.
Hello,
My previous post was based on this being a multibody part.
Since there's only an image, this could also be an assembly.
For an assembly, the end plate is an extrude from an elliptical sketch, with:
minor axis length = Pipe OD - wall thickness
major axis length = minor axis length/cos(pipe angle)
Mate the end plate face coincident to the pipe end and then select pipe and plate planes and mate them then coincident for the other two DOF.
Kevin
Kevin Chandler wrote:
Hello,
I'm assuming these end plates are welded onto the pipe.
If this is true, then you will need to:
- Leave some land for a weld bead
- Or 45° chamber the mating face of the end plate
If #1, then create a sketch on the 45° end of the pipe.
Convert entities on he ID & OD and change these ellipses to construction.
Create a construction line from the major apex of the ID to the major of the OD.
Do the same at the minor apex.
Create an ellipse with the major snapped to the midpoint of the major construction line and the minor snapped to the midpoint of the minor line.
This sizes the end plate at mid wall thickness. (You can opt to use fixed major & minor distances from the OD, too so set the weld bead size.)
..or place some construction lines as shown below...
...and sketch an ellipse, using relations to the construction line end points and center points to fully define it.
I would do my layout sketch like this - (use the construction lines to add planes)
Add the planes
Revolve
Shell
Cut through all
Add a sketch and covert the entities
Extrude
Hello,
Originally I was going to do an offset of half the wall thickness but I went straight to convert without seeing whether or not the lines would snap to the edges.
Kevin
keep it simple.
pick a plane, make a sketch, convert what you can offset. ect.
no need to make it complicated when you don't need to.
Are you using weldments?
It is a very, very strange solution.
1, Why you make planes? After cut you have it.
2. Pipe construction - extrude with Thin option is simply special that you have planes. You can extrude to plane in both direction and not must cutout.. If revolve - better us rectangle - its only one step.
3. If you make planes, why you don't use it for cutout?
Caps construction is ok. Like my
B.R.
Krzysztof Szpakowski wrote:
It is a very, very strange solution.
1, Why you make planes? After cut you have it.
If for some reason you would need to change the part into a Sheet Metal Part then it makes it much easier to add the end caps in an assembly, changing the part to Sheet Metal would eliminate the ability to add a sketch on the pipe ends.. ..
Might be strange, but I know it works and is "Robust"
Weldment. Indented bom set to detailed cut list. Insert bodies into new part if you have a s***** ERP system that doesn't recognize multi-body parts.
To everyone,
thank you very much, I picked pieces of several replies and came up with a solution.
There is a huge wealth of knowledge out there and you were all a help. I've used SLWKS for several years but not everyday and I am not as good with it as I should be by now.
Not to answer every question, but regarding weldments, I did not want this to be a weldment piece, I needed to use individual parts.
Simply drawing an ellipse is a good solution, but as well as ensuring something the correct size, I hoped to learn a simpler way to pattern the ellipse from the end of the pipe. Some of the answers helped me with that.
Finally, it was good to see several different ideas on the solution.
thanks again to everyone.
Mike Mc
Mike,
I see you've moved onwards but if you need guidance with moving forward with weldments we are here for you.
Are you familiar with the following?
Weldment Cut list as compared to Indented BOM?
Dissolving parts to show only cut list bodies in BOM tables?
Pulling cut list body properties into drawing notes?
Brian Graves wrote:
Weldment. Indented bom set to detailed cut list. Insert bodies into new part if you have a s***** ERP system that doesn't recognize multi-body parts.
That's exactly how I do it. No sketch mess.
RMC endcap "Insert into New Part" - Select export cutlist info to custom properties - Insert endcap part into the assembly and Badda Bing. Done.
Shows up in the assembly bom (without having to indent) and you've got an accurate flat pattern. Yay!
Master Sketch or SSP.
The sketch control everything. All parts reference only the Master. No circular reference
Everything in the sketch can be reuse.
I don't have problem with SSP. But rest. Look:
I think that this is faster and simply.
Faster, for 1 part. Maybe.
E... I say for John that its strange for me. For make pipe body John use 3 features (revolve, shell, and cut). You fink that 1 feature (extrude) is maybe faster?
Krzysztof Szpakowski wrote:
E... I say for John that its strange for me. For make pipe body John use 3 features (revolve, shell, and cut). You fink that 1 feature (extrude) is maybe faster?
Fastest way. Just draw an ellipse. Don't care if the pipe will change.
It became slower when pipe size change or cut angle change.
Add other parts and changes. All bets are off.
90% jobs will change with addition requirements add on to it.
So I'll just do Master for every job betting there will be changes.
I've never started in Master and regret.
But always regret I didn't start in Master.
When ever someone said "Its just a circle" never end up with just a circle.
1, Make sketch on cuting plane
2. In Scetch Use a cut edge - Convert Entities (inside or outside)
3. Add Extrude (if you need you can use pipe axis as extrude direction)
4. Make a coffee and smile
B.R.