Engrave logo on pipe

[Quick Karl]

Here is a problem that has me stumped

 

[Quick Karl]

I must have asked a tough question

I wish someone knew the answer...

 

[michael3130]

Hey Quick Karl,


I'm not getting my daily MCAd updates so didn't see your question.


1 - Offset the outer surface inward the depth you want your cut


2 - Insert a plane to draw the text which is outside the pipe.


3 - Extrude cut the text up to the offset surface.

 

[Mihail]

Hellow !


I think that the Michel's idea work. But not very well because you make a normal projected view from a plane shape to a cilindrical surface.


Assuming that the high of the text is not bigger than the diameter of the pipe, try that:


Make a new part. This part is"pipe" froma very thin sheet metal (0.1 or 0.01 mm). The cross section for new "pipe"is asmall line followed byanarc (180 degree is more than enoutgh) and the radius is a bit grater than your pipe. The small line create a small surface and this surfacewill be necesary for the UNFOLD feature wich ask youfor a fixed face.


Unfold this "pipe", make a cut with the logo sketch, then fold the "pipe".


Make an assembly with your pipe and the new one, and save it.


In the assembly make a plan as "parallel" as possible with the logo (now you can see well this logo) somewhere outside of your pipe, EDIT PART (your pipe) and EXTRUDE CUT. As plan for the sketch choose the plan you created.


Select all the logo's edges, convert entities, and exit from sketch.


in theEXTRUDE CUT feature managerchoose OFFSET FROM SURFACE option, set, as surface for offset,your pipe surface and... that is all to do.


Note that EXTRUDE CUT feature do not allow you to create multiple bodies, so you must work around your logo before try to cut the new "pipe".


I think that is easier to use surfaces instead a very thin sheet metal but I don't know (yet)to work with surfaces.


Hope you understand my english because I am not enough skilled to speak so much

You can email me at [email protected] and I'll send you the files I created to solve this problem.


Good luck !
Edited by: Mihail

 

[michael3130]

Sorry, I should have read the bit about you rotating the pipe about the x-axis during the engraving. Try Mihails suggestion though try and get the file from him as recerse engineering his model will help you to fully understand.


My method would have been fine if the pipe was stationary in relation to the cnc cutter.

 

[Quick Karl]

Hellow !


I think that the Michel's idea work. But not very well because you make a normal projected view from a plane shape to a cilindrical surface.


Assuming that the high of the text is not bigger than the diameter of the pipe, try that:


Make a new part. This part is"pipe" froma very thin sheet metal (0.1 or 0.01 mm). The cross section for new "pipe"is asmall line followed byanarc (180 degree is more than enoutgh) and the radius is a bit grater than your pipe. The small line create a small surface and this surfacewill be necesary for the UNFOLD feature wich ask youfor a fixed face.


Unfold this "pipe", make a cut with the logo sketch, then fold the "pipe".


Make an assembly with your pipe and the new one, and save it.


In the assembly make a plan as "parallel" as possible with the logo (now you can see well this logo) somewhere outside of your pipe, EDIT PART (your pipe) and EXTRUDE CUT. As plan for the sketch choose the plan you created.


Select all the logo's edges, convert entities, and exit from sketch.


in theEXTRUDE CUT feature managerchoose OFFSET FROM SURFACE option, set, as surface for offset,your pipe surface and... that is all to do.


Note that EXTRUDE CUT feature do not allow you to create multiple bodies, so you must work around your logo before try to cut the new "pipe".


I think that is easier to use surfaces instead a very thin sheet metal but I don't know (yet)to work with surfaces.


Hope you understand my english because I am not enough skilled to speak so much

You can email me at [email protected] and I'll send you the files I created to solve this problem.


Good luck !

Hello, Mihail,


Thank you for your reply -- I think I understand most of what you are suggesting I try, but I do not know what you mean "make a plan" (I highlighted your text in red above).


Also, if I understand correctly, this would still not be a precise model of the logoexactly as it would be engraved by CNC / G-code, but it would be VERY close.


I have a sinking feeling that I am in deep doo doo on this one - I can interpret the G-code for the logo (which I have), but I am lost on how to transcribe the movements onto the outside diameter of the pipe (around the circumfrence)...
Edited by: Quick Karl

 

[Mihail]

As "parallel" as possible: In your picture, Ox is axis for tube. Assuming that your text is along the pipe and the middle of the text is in plane Oxz, the plane "as parallel as posible" is Oxy. Or any plane parallel with this one. I say "as parallel as possible" because your text is on the cilindrical surface and a plane is... a plane.


I try to teach you HOW TO engrave the tube in SW. How to make this in realliti... I do not know. But, I think, youuse CNC machineto engrave the logo. And the CNC machine'ssoftware can read your SW file (maybe not .SLDPRT butin other format as .IGES)and perform automaticaly the task.


Sorry, I can not provide more help in this directtion.


Is quite simple, in math, to perform the projection for a line on a cilindrical surface. You must calculate the position for 2 points. But, if you are not an old chinesse, you can not calculate the projection for eachline or curvefrom your logo. So you must use a software to do this.


Good luck !
Edited by: Mihail

 

[JohnnyRetro]

If you have SW2009, use the "Project Curve" feature to
project a single, open or closed curve on a surfuce.You
might have to do this a few times if you have a complex
logo. When the curve is projected, you can use thse
"Cut-Sweep" feature to cut out the logo. Hope this
helps.

 

[Quick Karl]

As "parallel" as possible: In your picture, Ox is axis for tube. Assuming that your text is along the pipe and the middle of the text is in plane Oxz, the plane "as parallel as posible" is Oxy. Or any plane parallel with this one. I say "as parallel as possible" because your text is on the cilindrical surface and a plane is... a plane.


I try to teach you HOW TO engrave the tube in SW. How to make this in realliti... I do not know. But, I think, youuse CNC machineto engrave the logo. And the CNC machine'ssoftware can read your SW file (maybe not .SLDPRT butin other format as .IGES)and perform automaticaly the task.


Sorry, I can not provide more help in this directtion.


Is quite simple, in math, to perform the projection for a line on a cilindrical surface. You must calculate the position for 2 points. But, if you are not an old chinesse, you can not calculate the projection for eachline or curvefrom your logo. So you must use a software to do this.


Good luck !

Mihail,


I tried your suggestion, and the result looked GREAT while the part was flat... but as soon as I "re-folded" the part, the logo disappeared????

 

[Quick Karl]

If you have SW2009, use the "Project Curve" feature to
project a single, open or closed curve on a surfuce.You
might have to do this a few times if you have a complex
logo. When the curve is projected, you can use thse
"Cut-Sweep" feature to cut out the logo. Hope this
helps.

It is starting to look like this logo is going to be one time-consuming excersise...


I guess I am going to have to get the calculator out and start deciphering the G-code for the logo and do the 'projected curve' thing -- and for this logo it will probably take 2-weeks to do.


I have the G-Code as a txt file, and a dxf.; now I guess it's hours of work to get it done.
Edited by: Quick Karl

 

[Mihail]

Quick Karl, do not FLAT the sheet then UnFLAT.


Use theese steps:


1) Make the sheet


2) UNFOLD the sheet. "UNFOLD" is a command from the SHEET METAL toolbar. It is not the same command as FLAT command.


3) Cut the logo.


4 FOLD the sheet. This is OTHER command (and OTHER button, of corse) from the METAL SHEET toolbar.


Using this steps, you have the logo on your new "pipe".


Then follow the steps from my first post.


Good luck !

 

[Quick Karl]

Mihail,


I DID use the "unfold" and then "fold" tools from the sheetmetal toolbar - when I "fold" the part after getting the logo on it, the logo just disappears!

 

[Mihail]

Sorry, I do not understand what you are doing wrong.


I work exactly how I teach you and all is ok. Again, if you email me, I'l send you the files. I use SW 2009.

 

[Dynamica]

OK,
The easy way to do this is with the "WRAP" feature.

This feature only works on flat, cylindrical, or conical solid feature faces (Except scribe works on surfaces). The sketch also must be a closed profile.

1-create a plane parallel to a plane that is tangent to the conical or cylindrical face.

2-sketch on the newly created plane your design. You can also import a DXF/dwg file on this plane ie. logo.

3-select insert>features>wrap.

4-Select your face to wrap the sketch about. enter your depth. select your source sketch (the one you just created/ imported)

5- Now you can select emboss(extrude), deboss(cut), Scribe(make parting lines to delete faces)

I tried to upload pictures but it isn't working. If you email me i will send some screen shots.

Cheers, Tim

 

[Mihail]

Fine tool. Thank you, Dynamica !