Printable View
Can anyone tell me if (and how) can specify the entry/start point for a toolpath, especially when using Boundary Curves milling?
For example, if I draw a rectangular selection around an object, it will begin the toolpath on one side. What if I want it to start on the opposite side? Can I do anything to change the starting position, short of mirroring the object and using that as a model?
Thanks!
I assume that madcam is using rhino curve direction to know where the tool path starts and ends . So you might try flip the curve start direction in rhino.
The CrvSeam command (Curve > Curve Edit Tools > Adjust Closed Curve Seam) allows relocating a seam on a polyline, or any curve for that matter. When the command is started, an arrow is placed at the current startpoint, pointing in the polylines direction. Click and drag that to the desired startpoint. The ‘Flip’ sub-option will change the direction of the polyline.
I thought curve seam or direction command would do it too. However, it doesn't. As a simple test, I drew a rectangular boundary curve and then used these commands to place the seam at various parts of the rectangle, as well as flipping the direction of the curve. The starting and ending point are always the same, so it seems that madCam is ignoring this property.
Do you think it would be useful to define a point in your model so that madCAM starts as close to that as possible? I know this is something we've had in WorkNC forever, and it's pretty useful for making the toolpath start where you want. It could be something as simple as a prompt to define the start point for certain types of paths. That start point could be a point that you place close to the place you want the path to start. Or it could be any OSNAP to a feature of the part. I would think that it's closed pockets or curves that would benefit from this the most, as open features generally are good to have the path start on an end or edge.
Does this sound reasonable, and useful?
Dan
I think it would be useful to have an option for a starting point for sure. In my line of work (jewelry modeling), there is a fairly specific order to cutting the models because of the fragility of the material. So, being able to instruct to cut the furthest away from the support and towards it would be highly beneficial.
I just noticed in madcam there is a change curve direction button .... Is that the one you tried?
Was this issue ever resolved? I'm in exactly the same boat as Helios. I'm cutting wax for jewelry and it seems no matter what I do, madCAM starts cutting from location on the wax closest to the supports (i.e. nearest to the rotary table where the wax is in the holder). I'm using 5-axis from boundary curves. I've tried reversing the curves both using the madCAM tool and Rhino flip/ dir commands. I've tried moving the model, flipping the UVs of the model surface, scaling to -1, mirroring the curves and cutting from the opposite cPlane but nothing seems to work.
Perhaps I'm missing something obvious. Can anyone help?
Thanks.
Problem solved. The trick is to mirror the surfaces (source) being selected for tool path calculation. At least this trick works for symmetrical geometry. I also found it worked to mirror the surfaces being selected for tool path calculation in the Z-direction, generate the toolpaths, and mirror the toolpaths in either the x or y axis, mirror again in the z-axis, and rotate 180 degrees in the z-axis.
I'm updating my answer with a more clear step-by-step explanation since I just ran across the problem again and I couldn't *quite* remember exactly how I fixed this the first time. So I documented this for myself and I thought it would be nice to share. It's a bit of a painful workaround if you have a custom CPlane, but it works for me.
FYI, I'm using a 5-axis machine for wax cutting (jewelry), so my axis of revolution is in the Z-axis and the solution below is based on that orientation:
A. To reverse the direction of a toolpath:
1. _Mirror (with the Copy flag set to yes) the surfaces, polysurfaces, and/ or meshes (and boundary curves if applicable) being selected for tool path calculation in the world Z-axis (front camera).
2. Generate the toolpaths.
3. _Mirror the toolpaths in either the X or Y axis (i.e. front or right camera, Copy flag in the _Mirror command set to no).
4. _Mirror again in the Z-axis (i.e.front camera, Copy flag set to no).
5. _Rotate 180 degrees in the Z-axis (i.e.top view).
B. If one is generating the toolpaths from a custom CPlane (for example, in order to use 5-axis From Boundary Curves), the custom CPlane will need to be mirrored as well in order to correctly generate the toolpaths:
1. Draw a plane (_Plane) in the viewport set with the custom C-Plane you wish to mirror.
2. _Mirror the plane in the world Z-direction (front camera, Copy flag set to no)
3. Create a new viewport (_NewViewport or Viewport Menu > Viewport Layout > New Viewport).
4. Name the viewport in Named Views to something clever (_NamedView or Viewport Menu > Set View > Named Views...)
5. Use _OrientCameraToSrf (in the Set View toolbar, has a camera icon) to set the CPlane to the plane you created (pay attention to the surface direction and use the flip flag as necessary to make sure the camera is oriented the correct direction).
6. Use the _CPlane command and use the View flag to 'Set CPlane to view' (CPlane menu, icon with an eye).
7. Delete the plane.
8. From here you can follow the steps in Section A above to mirror the source (and boundary curves if applicable).
9. After you're done, you can close the viewport (_CloseViewport or Viewport Menu > Close Viewport) and delete your duplicated/ mirrored geometry and curves.
SOLVED: Entry/start point of tool path for MadCam.
Hello all. Like MANY of you I have had a Hell of a time with my entry/start points in MadCam. I found a much easier solution than anything else I've seen. It's so simple and you can tell MadCam EXACTLY where you want to start cutting. All you have to do is draw in a lead in (and lead out if you desire). Or, just make a small break in your curve and MadCam will start and stop right there every time.
In this first picture, MadCam "chooses" where it wants to put the entry/starting point. It seems no matter what you do, you can't move where the tool will start...
Attachment 445104
The fix is so simple... In this picture I made a gap in my curve and drew in a lead in and a lead out. When you generate your toolpath, MadCam will start and stop right there everytime! Awesome! Just be sure to create an offset the radius of the tool and select "cut on curve". Because of the break that is made in the curve, Madcam no longer recognizes what is the left and right side of the curve. Meaning that it doesn't know whether it is conventional cutting or climb cutting. If you don't compensate for this, your part will not come out the correct size. If this doesn't make sense please respond back to me and I will try and clarify.
Attachment 445102
In this picture, we are doing the same thing. Except I eliminated the lead in and lead out. The gap I made in this picture is huge. You can make the gap much smaller. I only made the gap large so it's easy to see what is happening. Again, MadCam is no longer "choosing" where the entry/start point is. We now have complete control over this, using this method. Please don't forget to create the offset for the tool you're using and select "On Curve" for the tool offset.
Attachment 445106