help to finish a multiple surface cavity

[Mike Mattera]

Not every part or every toolpath lends itself to creating arcs or smooth filtering. On some parts filtering might not be the best thing to do. Filtering makes lots of moves into fewer moves. So on some geometry it might create more choppiness (is that a word?). It might be better to have 10,000 points if they follow the surface more exactly. The problem with choppiness could be in the positioning of the machine. If the drives aren't tuned right, you could be getting a jerking motion, rather than a smooth interpolation.

As for the location of the videos that cover Filtering....

3D overview - Lesson 2 = Tolerance in general

ToolPath Info - Roughing - Lesson 7 = Complete description on the concept of filtering, ratios, arc filtering, One Way direction, Arc limits, plane selection.

ToolPath Info - Finishing - Lesson 1 = Filtering for arcs. XZ plane.

After those explainations, almost every part example uses the Total Tolerance/Filtering function for the toolpaths. Each with some small mention of how it will apply to that particular part.

Remember: the toolpath type and cut direction determine the efficency of the filtered result. Contour cut, cuts in planer slices, giving you XY arcs. Parallel cuts in X can give you arcs in YZ. Parallel in Y can give you arcs in ZX.

Is your post outputting 3 places or 4 places ( X.123 or X.1234)?

Hope that helps,

Mike Mattera

[maxine]

The test part I am trying to learn on is a simple cylinder with a cylindrical hole cut into a boss in the middle. I was trying to pocket it out, then profile the outside. That seemed to me like it should be the ideal part for filtering arcs. I have been using 2:1 filtering as the CD suggests. I have tried total tolerances from 0.02 up to as tight as the program will let me go without giving an error (I think that was 0.00005 maybe?). I have checked one way filtering and arcs in xy only boxes. The machine I am learning on is a new Haas TM1 and it cuts a nice smooth arc if I just hand program one in. If I use the conversational program option and ask it to pocket out a hole the same size and depth as one of the ones I was trying to use Mcam for on my part I also get a very nice smooth hole. I am using the generic Haas post that was with X. I will have to check to see if it is outputting 3 digits or 4 after the decimal. I am not at the shop today so I can't check until tomorrow and I only have access to mcam nights and weekends. So it seems to me it has to be something I am doing wrong in the CAM. I have watched those sections of the CD over and over but I must be missing something. So can I ask a favor? Is there a way I can send you the part file and ask you to take 10 minutes sometime when you are free and just quickly program a couple of the ops so I can see how you did it. Then I can duplicate that here and try running it on my machine? I really wanted to get good at this and try to make it a career someday but I am so frustrated I am ready to give up tyring to learn it...

[Mike Mattera]

send it to me. I'll take a look at it.

Mike

[Derek Goodwin]

surface finish is not only controlled by filter tolerance or even surface tolerance. If you get facets on arcs that are created by circular interpolation (2D Arcs) then the problem may be in the machine tool (gibbs and backlash.) Surface finish problems in 3D can be due to toolpath type. Surface finish contour will produce a good finish on near vertical walls, but a poor finish on near horizontal walls. parallel will have the opposite effect. This is because some paths use step down for defining the kerf and others use step over. Scallop will give you an even distance between cuts, as will flowline. Sometimes you will need to combine several different toolpaths, controlling the cuts through boundaries and cut depths to get the desired effect. Each geometry has it's own complications, so there is not one method to fix all. HTH

oops just read the rest of the posts. I'm not sure surface finish toolpaths are even what you need for this part.

Mastercam training Online http://eapprentice.net/

[manuelc149]

i am milling a part that has a 1 deg draft using surface finish scallop. the tool path is going all around the part from bottom to top,( exept the beging it starts at the bottom takes about two complete passes then gose to the top then back to the bottom ). my major problem is why is it zizgzaging in the middle of the part leaving me gauges?

[Derek Goodwin]

It may be easier if we can see the file. How about surface finish contour? It will go all the way around the part consistently, from top to bottom regardless of surface irregularity

Mastercam training Online http://eapprentice.net/

[Derek Goodwin]

Originally Posted by cadcam You can use cut depths in rough pocket to start lower and start at the bottom. review picture.

CAD/CAM, this photo reminds me that using depth of cuts absolute often leaves more leftover material at the bottom of the cavity, whereas incremental doesn't. I have played with cut depths, but that doesn't solve it. Any idea why? I have wondered if this is a bug.

Mastercam training Online http://eapprentice.net/