Author Topic: Trying to rotate a polyline to YZ axis to machine but it's not coming out right  (Read 359 times)

Offline tlmkr38

  • Ewok
  • *
  • Posts: 16
    • View Profile
we have a profile that we need to mill in the YZ axis. I can draw it then import into CB but once I start rotating it when I get where it should be the profile changes. I want to use a ball endmill and step it over for the width of the part. I can hand code it but want to be able to use CB for making the code if possible. I am attaching what I am wanting to mill and what CB come up with when i rotate everything. It's something simple I'm sure but I cant figure it out.

First file ( Bottom form) is the profile looking from the side view. I want to be able to use a 0.5 ball endmill to mill this profile about 6 inches wide. When I turn the profile in CB it makes the radius's go off to the sides instead of running true on the axis. 2nd photo shows after rotating it in CB.

 if someone can tell me what I'm doing wrong I would appreciate it. I have the Stl file to machine with the 3d option but I haven't figured out how to just cut the top using that and not having the mill do down on the front and back sides yet.

Offline EddyCurrent

  • CNC Jedi
  • *****
  • Posts: 5065
  • Made in England
    • View Profile
The dxf has Arcs and Lines, select them all then Edit->Join, to produce a Polyline.
Now select the Polyline then, Edit->Polyline->Remove Arcs, use a tolerance value to get a line within the required accuracy (try 0.01  or smaller) as it will now consist of multiple small sections joined end to end.
Rotate the polyline and it should now look okay.

Another way is to;

In Tools->Options->Spline  to Polyline tolerance, set a value of 0.001 or smaller. You must save these settings and restart CamBam
Draw the shape as a Spline
Rotate the Spline as required
Select the Spline then, Edit->Convert To->Polyline.


Filmed in Supermarionation

Offline dh42

  • Administrator
  • CNC Jedi
  • *****
  • Posts: 6892
    • View Profile
    • Cambam V1.0 French Doc
Hello

Quote
Select the Spline then, Edit->Convert To->Polyline.

A spline on XZ or YZ plane can be used "as is" with an engrave mop, no need to convert it to polyline.

++
David

Offline tlmkr38

  • Ewok
  • *
  • Posts: 16
    • View Profile
I have to make it a polyline before bringing it into CB? I opened the dxf then converted it in CB but if needed I can do it before. What I didn't do though is remove the arcs. I'll try that...

Offline lloydsp

  • CNC Jedi
  • *****
  • Posts: 8649
    • View Profile
Timkr,
My opinion is that he was talking about doing all of that within CB.

David,
I'm curious about why some of the splines turned 'wrong' when rotated.  I've seen that before, but because I'm always in a hurry, figured-out different ways around it.

Could joining and converting to polyline perhaps fix that?

Lloyd
"Pyro for Fun and Profit for More Than Fifty Years"

Offline tlmkr38

  • Ewok
  • *
  • Posts: 16
    • View Profile
I think he was also now. I went in and reloaded the DXF and and converted and took arcs out and it rotated like it should. can now use the engrave to get the toolpath and then just loop it side to side as needed. thanks!!!!!

Offline dh42

  • Administrator
  • CNC Jedi
  • *****
  • Posts: 6892
    • View Profile
    • Cambam V1.0 French Doc
Hello
Quote
David,
I'm curious about why some of the splines turned 'wrong' when rotated.  I've seen that before, but because I'm always in a hurry, figured-out different ways around it.
I never have had problem when rotating splines ; what we can see is that if we convert a spline to a polyline, if the spline is on XY plane, it is converted to a polyline that contain arcs, but if it make any angle with XY plane, it is converted to polyline that contain only small straight segments.

It is with polylines that contain arcs that we can't rotate them without to have deformed arcs

++
David