MIRRORING ENTIRE DRAWING WITH TOOLPATHS?? IS THIS OK?

[AvB]

Hi,
I am a fairly basic amateur, having played intermittently with Rhino, Madcam and a fairly good solid accurate 3-axis router table for 3 years now. I have had pretty good success making model aircraft moulds, but with plenty of head scratching and stuffups along the way. I’m always cutting Corian or Freestyle (acrylic or polyester solid surface benchtop materials). So I have a reasonable amount of experience but there are a lot of basics I don’t know and I tend to go much too long between jobs and forget half of what I’ve learnt.

I am currently cutting negative moulds for a nicely designed dynamic soaring sailplane fuselage. It involves cutting pockets and using inserts to get good shapes for fillets and steps, so there are a lot of toolpaths and uses quite a few different cutters to get into fiddly areas and shapes. It's quite a big job getting the toolpaths sorted. I have almost completed the first side which will then be taken off the table and I’ll start on the other side.

MY QUESTION IS:
The two fuselage halves are complete mirror opposites of each other. Can I save time and effort by mirroring the entire drawing including the hundred or so Madcam toolpaths, and then re-selecting and postprocessing them appropriately?

I know that this works for more simple things but haven’t tried it for a more complex shape. My thinking is that the only issue would be that any climb toolpaths will now become conventional, but I tend to think that wouldn’t be a problem.

Any advice or warnings very much appreciated.

Thanks, Andrew

Similar Threads:

• Need Help!- Mirroring Toolpath
• mirroring toolpaths in NX7
• Problem- Mirroring
• Mirroring with Mach
• Which Software allows direct drawing of toolpaths?

[Dan B]

You have to be careful. Transformations work well for madCAM paths except for mirroring. You may find when you mirror that the clipping planes get inverted.

That's the bad news. The good news is that you don't have to do that, especially if it's okay to climb and conventional cut in your material. We find that we restrict climb cutting only to steel. Even aluminum works well if you mix your cutting styles. What you should do to save a lot of repetitious work is to create a set of mirrored post-processors. Depending on your controller, it could be as easy as adding something like G51.1X0 (if you mirror in the X axis) or for Heidenhain CYCL DEF 8. But even if your controller doesn't support mirroring you can still accomplish this with a very simple post hack as shown below:

*SCALE_1*
-1 <<< Just change the scale to negative for the axis that you want to mirror.
*SCALE_2*
1
*SCALE_3*
1
*AXIS_1_CHAR*
X
*AXIS_2_CHAR*
Y
*AXIS_3_CHAR*
Z

I also find it beneficial to add a comment line so that the mirrored code is easily identifiable:

N"lnbr" (This mirrored in X code is from madCAM for the Doosan)

Almost everything we cut has symmetrically opposite handed parts, so we've had a lot of experience with mirrored toolpaths. Even if you are doing multi-axis work, it's still possible to mirror your paths with a couple of simple post changes.

Hope this helps,

Dan

[AvB]

Great advice thanks Dan. I'm really surprised that mirroring could invert the clipping planes! Seems strange when everything else in the drawing would mirror only around the Y, but I don't understand the Madcam technicalities. I'm not sure if I'll go that way at the moment as it might do my head in if I needed to go back to the drawing to revise any toolpaths ... I'd probably need to practise it on some test shapes first.

[Dan B]

It's a bug. It wasn't intended to be that way. Maybe it will be fixed in the next service release, I guess time will tell.

[AvB]

Hey Dan, if I did try mirroring everything, is it apparent if the clipping planes invert themselves? Or is the problem hidden somehow? I would like to try it and see if it works - but I'd need to know whether it's clear that it fails. I don't want to take risks with this one. , Or, is it an absolute definite that the clipping planes will invert? If so I won't try.
Cheers
Andrew

[Dan B]

Hey Dan, if I did try mirroring everything, is it apparent if the clipping planes invert themselves? Or is the problem hidden somehow? I would like to try it and see if it works - but I'd need to know whether it's clear that it fails. I don't want to take risks with this one. , Or, is it an absolute definite that the clipping planes will invert? If so I won't try.
Cheers
Andrew

The mirrored toolpath may shift out of location in the Z. That is what I have observed. Its always been a substantial amount the times that I saw it happen.

[AvB]

Thanks very much Dan, I'll check.

[svenakela]

That must be something new, I've been mirroring paths quite a lot in the past.

[AvB]

Timely reply Sven. Just right now I've taken the finished drawing of the left side mould, selected everything (drawing and all Madcam toolpaths) and mirrored them. I went through the toolpaths selecting them one by one "select objects" and it shows the paths on both sides, and I can see that they are at the same Z level and all appear to have mirrored OK. So I deleted all of the original (left) side and am going to start work using the mirrored toolpaths on the other side tomorrow. Fingers crossed.

[svenakela]

[warrenb]

Depending on your CNC controller you might be able to mirror it with a simple gcode. For example it is G51.1 (axis) on Fadal

[Dan B]

I'm glad it worked out for you, but I would be careful. We didn't see it every time either, but we did see it shift more than once. When I discussed it with Joakim, he was the one that told me there is a bug that inverts the clipping planes. Mirroring using one of the methods I described above works for us 100% of the time.

Dan

[AvB]

Hmm, well I've just had the first problem. I mirrored some of the first toolpaths with no problems. But I mirrored some finishing Z and planar cuts for the fuselage cavity which use an 8mm ballnose cutter, and despite the toolpaths being in exactly the right position on the drawing, it is running the cutter 4mm above the correct position ... I assume because it's somehow treating the cutter like a square end mill, not a ball nose. The ball nose toolpaths are centred at the centre of the cutter radius, not at the tip. I tried re-selecting the 8mm ballnose cutter as the tool, then re-post processing, but the result was the same.

Anybody have any ideas on whether there's some setting that needs to be checked?

[Dan B]

This is why we don't mirror toolpaths. Follow my earlier suggestions for alternative ways to mirror your part.