Need help in understanding surface toolpaths (countor and flowline)

[beginner1977]

Granted that I am a beginner in using mastercam, I need some help in understanding the methodological approach needed to implement surface toolpath (rough and finish).

As case of study I have got a set of surfaces describing a 3D open contour.

As first operation, I have used surface rough contouring by leaving a stock of 0.3mm and using a boundary 2D chain as containment boundary (the tool is restrained to path internally the containment boundary). The result is that the toolpath is enough even and smooth and follows smoothly the drive surfaces pattern selected.

As second operation, I have used surface finish countouring by selecting the same drive surfaces and containment boundary used for roughing operation. I have set up the stock to 0.0mm and kept the rest of default parameters. The result is awful. The toolpath doesn't follow smoothly the drive surfaces and presents a lot of "break and retract motions". If I set up the stock to 0.02mm the toolpath is almost smooth and acceptable but I don't understand why I have to introduce a fake stock of 0.02mm to have the toolpath almost acceptable. My goal is to have a toolpath which follows smoothly the drive surfaces selected (without fake stock value) since these surfaces are part of finish machined 3D geometry.

I also need help in understanding how to use rough and finish flowline toolpaths properly.

How does Mastercam interpret the drive surfaces as flowline ruled?

Sometimes I get an error message telling me "Surfaces selected not aligned or ruled" also in case the surfaces selected, at first sight, look like flowline ruled in the same direction.

Is there a tool in Mastercam that could make a checkout of drive surfaces giving a response about inner flowline direction of surfaces checked and giving the chance to modify such direction?

 

Any suggestions to help me in understanding how Mastercam approach what highlighted above?

 

Are there some exhaustive tutorials clearing out these doubts?

 

I will be really thankful.

[Rotary Ninja]

Here are a couple threads discussing the contour toolpath...

http://www.emastercam.com/board/index.php?showtopic=70259

http://www.emastercam.com/board/index.php?showtopic=70514

[NOTW Programmer]

There is the Mold PLus add-on which allows you to change the UV on surface and make them all the same. http://www.moldplus.com/

[Rotary Ninja]

How much is that addon?

[MotorCityMinion]

I'm guessing that the part your trying to cut with SF Contour has faces around the perimeter with different slopes and or edge geometry at the top. The reason the tool is hopping around is because it is trying to cut tangent to those faces at the top 1st. As you've found out, extending those surfaces above the part will smooth it out some. Here's how to smooth all of it out. Knowing the radius of your tool, extend all those faces well above the part by at least the tool radius.

EX: .06 rad on tool, extend your surfaces by at least .07.

 

To extend them, copy the original surfaces to a new level. Use the untrim feature on every face. Extend all those faces well above the part. Now, trim them all to the same plane. Next, extend those surfaces so that they go through the adjacent surface completely. Trim those surfaces to the adjacent surface or edge curves that you create. If the top edge has a rad on it, you will have to get creative and create vertical surfaces in that area that will work. When your satisfied with the results, look at the surfaces closely and make sure they do not overlap. Now when you program the toolpath, include all those newly trimmed surfaces and use the depth limits in the toolpath, of course setting the top to Z0.0.

 

You can also use the edges of the surfaces, create curves around them, offset the curves inward by a amount greater than your tool nose radius then extrude new faces upward. This method can produce dummy drive surfaces much quicker depending on the geometry. BTW, using dummy drive surfaces can be an excellent way of controlling how a tool enters and exits the cut without using directional controls or tangential line length extensions, which can easily crud up a pristine tool path.

 

If this sounds like to much BS, set your depth limits to start at a negative value that is greater than your tool radius (for SF Contour) and keep adjusting the depth until you get uniform results. Program those upper faces using a different strategy, say blend , flowline, parallel and so on also using depth limits. Using SF Contour, your going to get different surface finishes on the faces depending on the slope anyway. In most cases, no single tool path will give you uniform results everywhere in the same operation. If your going after sweet looking finishes, toolpathing the faces individually, piecing the program together with multiple operations may be your best/only option.

[Rotary Ninja]

If you could supply a pic it would be easier to give you some ideas for toolpaths. Use the Windows snipping tool if you must.

[Reko]

If you are trying for a uniform finish across multiple surfaces, then Surface/Finish/Scallop is the path you want.

 

Sometimes, you need to break area's down and attack them separately... like steep walls first, then flatter surfaces together last.

 

Flowline only works well on a single uniform surface, in my experience anyway.

 

I like Surface/Rough/Contour, but for a finish, like I said, Scallop is the way to go.

[Tyler Robertson]

scallop or blenddd