Scam post? rotary function in Sheetcam.....
Scam post? rotary function in Sheetcam.....
http://www.plasmaspider.com/viewtopic.php?f=3&t=5113
There is a feature used in this topic to wrap a 2d drawing around a tube with a given diameter using the 4th axis.
I can not reproduce this process in Sheetcam and I can not find the information in the manual.
How is Vmax549 (4th and 5th post in the topic) doing this?
I want to use this function for my tube notcher.
Hoping to find a explanation!
Jacala
The Netherlands.
There is a feature used in this topic to wrap a 2d drawing around a tube with a given diameter using the 4th axis.
I can not reproduce this process in Sheetcam and I can not find the information in the manual.
How is Vmax549 (4th and 5th post in the topic) doing this?
I want to use this function for my tube notcher.
Hoping to find a explanation!
Jacala
The Netherlands.
Hi jacala,
this is my solution :
#1 Copy the pp in the attached zip file to the posts-directory of Sheetcam
#2 Suppose your tube or column has a diameter of 100 mm then the circumference has a length of 100 * PI where PI is 3.14159
#3 SC uses the Y-value of your drawing for calculations so draw in your favourite CAD software a rectangle of i.e. 50 mm in X and 314.159 in Y
#4 Add some text or other shapes like I did in my example, export this drawing in dxf format and import it to SC
#5 Select in SC from the menu Options -> machine -> post processor the pp from #1
#6 You need to add 2 variables to make this pp work :
one named Diameter
one named Angle
where angle is set to 0 if the surface of your tube isn't conical
Both variables are case sensitive
#7 create an contour operation as usual and select the shapes you want to wrap
#8 start the pp by clicking on P in the top left corner and save the created file
This workes for me to create the attached files
Richard
this is my solution :
#1 Copy the pp in the attached zip file to the posts-directory of Sheetcam
#2 Suppose your tube or column has a diameter of 100 mm then the circumference has a length of 100 * PI where PI is 3.14159
#3 SC uses the Y-value of your drawing for calculations so draw in your favourite CAD software a rectangle of i.e. 50 mm in X and 314.159 in Y
#4 Add some text or other shapes like I did in my example, export this drawing in dxf format and import it to SC
#5 Select in SC from the menu Options -> machine -> post processor the pp from #1
#6 You need to add 2 variables to make this pp work :
one named Diameter
one named Angle
where angle is set to 0 if the surface of your tube isn't conical
Both variables are case sensitive
#7 create an contour operation as usual and select the shapes you want to wrap
#8 start the pp by clicking on P in the top left corner and save the created file
This workes for me to create the attached files
Richard
- Attachments
-
- Jacala.zip
- this zip file contains all files I used or created for this post
- (106.84 KiB) Downloaded 368 times
-
- the result
- Wrapped output.jpg (35.21 KiB) Viewed 9034 times
-
- the imported drawing in SC
- SC-Shot.jpg (60.88 KiB) Viewed 9034 times
Last edited by ArchieF on Tue Jul 02, 2013 8:34 am, edited 1 time in total.
First of all: What a great explanation and I owe you one!
I've installed the Post pr. and did exactly how you explaned.
I've got the processing figured out, at least I think I do.
I'm gonna fiddle with it because I'm hitting a little bump here and there. Still learning a lot.
Thanks and I'll be back in a few hours with some questions
I've installed the Post pr. and did exactly how you explaned.
I've got the processing figured out, at least I think I do.
I'm gonna fiddle with it because I'm hitting a little bump here and there. Still learning a lot.
Thanks and I'll be back in a few hours with some questions
MMM
for some reason I can export the file as g code but Mach 3 can't work with it.
When exporting the same file with pp mach3 plasma it works great.
When exporting with Minimum G-code no arcs post processor (edited) there is an error in the beginning of the G code when viewing in Mach3
Bad character used: N0020 new function
N0020: new function
N0030: new function
N0040: new function
I'm searching for an answer but found none yet!
for some reason I can export the file as g code but Mach 3 can't work with it.
When exporting the same file with pp mach3 plasma it works great.
When exporting with Minimum G-code no arcs post processor (edited) there is an error in the beginning of the G code when viewing in Mach3
Bad character used: N0020 new function
N0020: new function
N0030: new function
N0040: new function
I'm searching for an answer but found none yet!
- Les Newell
- Site Admin
- Posts: 3668
- Joined: Thu May 11, 2006 8:12 pm
That is due to a bug in the post. I would guess it was put there for testing purposes. Go to Options->machine->post processor and click on the 'edit post' button. Look for:
function OnNewOperation()
In that function you will find:
post.Text(" new function\n ")
Delete that line, save the post and try it again.
function OnNewOperation()
In that function you will find:
post.Text(" new function\n ")
Delete that line, save the post and try it again.
Hello Les!
That worked a charm! Thanks.
Mach is showing the correct part now, y axis is moving, Z axis is moving so now only A axis, that one doesn't do anything at the moment but also gives no reaction in mach3 when jogging A/4th axis stays 0.000
The G code gives the right data so there is a setting wrong in Mach, or at least I believe that is the problem.
The weird thing is that the ports and pins settings are correct and are enabled for Y, A and Z axis. Could have something to do that this pc runs only a demo version of Mach 3.
I'll try it tomorrow on the real machine and come back with the results.
Were getting there. A bit more learning and searching to do Thanks.
Edit:
Reinstalled Mach 3 and problem solved! Looks great and cant wait to start cutting tube!
That worked a charm! Thanks.
Mach is showing the correct part now, y axis is moving, Z axis is moving so now only A axis, that one doesn't do anything at the moment but also gives no reaction in mach3 when jogging A/4th axis stays 0.000
The G code gives the right data so there is a setting wrong in Mach, or at least I believe that is the problem.
The weird thing is that the ports and pins settings are correct and are enabled for Y, A and Z axis. Could have something to do that this pc runs only a demo version of Mach 3.
I'll try it tomorrow on the real machine and come back with the results.
Were getting there. A bit more learning and searching to do Thanks.
Edit:
Reinstalled Mach 3 and problem solved! Looks great and cant wait to start cutting tube!
one day later a weird problem
Hello!
Today I was tinkering again but while I changed nothing there is a weird fault in the G code.
For some reason the third line of G code is not functional and gives the A axis the command to keep rotating until it reaches a 20 digit number, so that could take a while .
You can see the attachement with the fault on line 3. I've tried a new different DXF but that changes nothing.
When I delete the line of G code it works just fine like yesterday. So, what could be causing this weird G code value?
Today I was tinkering again but while I changed nothing there is a weird fault in the G code.
For some reason the third line of G code is not functional and gives the A axis the command to keep rotating until it reaches a 20 digit number, so that could take a while .
You can see the attachement with the fault on line 3. I've tried a new different DXF but that changes nothing.
When I delete the line of G code it works just fine like yesterday. So, what could be causing this weird G code value?
- Attachments
-
- Example with weird A rotations2.tap
- (14.39 KiB) Downloaded 331 times
In the attachment is the file. But it happens in all the files, also when I make a brand new file.
You can see the attachment, there are 2 files with both the problem.
It came up without changing anything to the settings so there is probably only 2 options: I'm doing something wrong or there is a bug.
You can see the attachment, there are 2 files with both the problem.
It came up without changing anything to the settings so there is probably only 2 options: I'm doing something wrong or there is a bug.
- Attachments
-
- Flat pattern cam klaar.dxf
- (33.77 KiB) Downloaded 286 times
-
- meter 12 grolsch amsterdammers.DXF
- (212.79 KiB) Downloaded 288 times
No problems here with your files.
Did you set the variables correct ?
Looks to me as if your startpoint is pretty far away from the part itself.
How far away from X0 / Y0 is your drawing ? What are the values at the bottom of the SC window in the X and Y field ?
Richard
Did you set the variables correct ?
Looks to me as if your startpoint is pretty far away from the part itself.
How far away from X0 / Y0 is your drawing ? What are the values at the bottom of the SC window in the X and Y field ?
Richard
- Attachments
-
- Bottom.jpg (11.94 KiB) Viewed 8946 times
-
- meter 12 grolsch.jpg (212.62 KiB) Viewed 8949 times
-
- Flat pattern.jpg (127.26 KiB) Viewed 8949 times
In the attachment is the faulty code.
Thanks for helping me. Weird that something is changed in a day that gives this error.
Good luck checking it out!
Thanks for helping me. Weird that something is changed in a day that gives this error.
Good luck checking it out!
- Attachments
-
- faulty third line of G code.job
- (7.41 KiB) Downloaded 340 times