Surface contour

[Thoob]

Is it just me or is this the dumbest surface toolpath Mastercam has? I have a part that I need to put a bevel on 3 surfaces. 2 of the sides are straight (0 and 90 degrees) and the other one is a 14" radius. See picture. What toolpath should I use here? When I use a surface contour, the path goes all over the place, nothing smooth about it and it keeps rapiding up in random spots. Little help please? lol.

 

[pip]

If you change your gap settings, that should keep the tool more in contact with the material. Less up and downs. Or better still, the Hispeed waterline toolpath..

[Thoob]

I used a flowline on it and it worked. I thought the flowline was for straight edges only? It works great on the radius. Or is it cause its such a big rad?

[The Chipmaker]

Yes change your gap settings for the contour, but is it a vertical (no draft) wall? Waterline and/or flowline with both work, but you will still ahve to change gap settings.

[htm01]

flowline is good for single surface, with more you may have problems with them lining up

[Thoob]

Ok cool. Thanks guys.

[NOTW Programmer]

Is it just me or is this the dumbest surface toolpath Mastercam has? I have a part that I need to put a bevel on 3 surfaces. 2 of the sides are straight (0 and 90 degrees) and the other one is a 14" radius. See picture. What toolpath should I use here? When I use a surface contour, the path goes all over the place, nothing smooth about it and it keeps rapiding up in random spots. Little help please? lol.

You need to use a boundary when you use contour, and definetly use gap settings to reduce retracts; I suggest you to use follow surface as your transition method.

[Rotary Ninja]

The surface finish contour toolpath works fine for this type of surfacing. It's all the the settings.

 

You could try...

 

Using a .500" Ball endmill, setup your tool and the surface parameters. Then move to the finish contour parameters tab.

 

Set the tolerance to .0005".

 

Direction of open contours set to zigzag.

 

Set transition to follow surface.

 

In the lower left check "Order cuts bottom to top". The reason I prefer this is the center of the ball never does any work. You will find you usually get a much nicer finish this way. Just watch for the initial plunge to be outside the material.

 

Click the cut depths button and check Absolute. Right-click in the minimum field and select "Z coordinate of a point". Click the top of your chamfer. Do the same for the maximum depth but select the lower breakout of the chamfer. Whatever value you get by clicking the lower line of your chamfer type after it -.250 and hit enter. You are using a 1/2" ball compensating to the tip so you need to lower this maximum depth setting by -.250" to get the breakout of the ball to cut even with the breakout of the chamfer. These settings will cut air at the beginning and the end of the toolpath since this is a chamfer. But not knowing the angle I can't give you exact figures.

 

From there click the gap settings. Click distance and set this to 1.000".

 

Click the advanced settings button and select "only between surfaces (solid faces)". This will keep the toolpath from wanting to wrap around the end of the part.

 

HTH.

[Oscar R.]

Am I missing something here?

From the pictures this looks like a regular chamfer to me.

Is this bevel ramping up, is it larger on one end than the other, or have a concave along the surface?

 

It just seems to me from the pictures that it would be easier to use a chamfer mill on a contour toolpath to make it.

[Rotary Ninja]

Am I missing something here?

From the pictures this looks like a regular chamfer to me.

Is this bevel ramping up, is it larger on one end than the other, or have a concave along the surface?

 

It just seems to me from the pictures that it would be easier to use a chamfer mill on a contour toolpath to make it.

 

I thought of this too, but rather than ask the question "Is this just a standard chamfer?" I chose to help him better understand the contour toolpath. I assumed he wouldn't use a surfacing toolpath unless he actually needed to.

[MotorCityMinion]

From the top view pictured, that bevel is fairly steep. I have limited access to chamfer mills and by the time I've completed my Lewis & Clark, looking for the tool, getting one ground up or ordering it, the program is written and ran. Flowline on that surface for sure. Now if I had a production run of those parts, new tools would be the way to go, but for one or two parts, I know I'm not getting out of that chair for tooling.

[Mick]

One hint when doing Surface Finish Contour: I've found if you use a boundary that is right on the surface edge, you tend to get a lot of hops up and down, and the gap settings do little or nothing to change that. However, if you use the Boundary setting set to On, rather than Inside, the "hops" are either removed completely, or reduced considerably. I experienced this just the other day, and it frustrated the heck out of me, until I tried the on setting.

[Rotary Ninja]

I wouldn't use a containment with this contour. Here is what you get with the settings I listed above...

[Mick]

My suggestion was a general hint for containments

[Rotary Ninja]

Ah, I see that now after re-reading it.

[Thoob]

That looks great. Thanks guys.