Not making smooth arcs!

[mattfurches]

Using mastercam x5 with a haas vf2 mill and a 4th axis. Im using the generic haas 4 axis vmc post processor. When the mill is making a 2d curve, just a simple arc, the face looks like a series of short lines. Almost like the facets of a diamond instead of one smooth face. Is this coming from my post or what?

[WallyL7]

It would sure be helpful if you could post your mcx file and the code. Is the code arcs or line segments? Is it a spline or actual arc? etc...etc...etc...

[mattfurches]

Here is a snippet of the code. It is a 3d solid model imported as an ipt file from inventor. And yes the rounded shape was originally a spline. ANy help would be appreciated. I cant figure out how to post the mcx file.



N9980 Z-.4933 F8.
N9990 Y-1.1 F20.
N100 G2 X1.45 Y-1.37 I-.27 J0.
N110 G1 X.2
N120 G2 X-.07 Y-1.1 I0. J.27
N130 G1 Y-.5961
N140 X-.0921 Y-.5966
N150 X-.158 Y-.6043
N160 X-.2462 Y-.6215
N170 X-.3587 Y-.6508
N180 X-.4993 Y-.6954
N190 X-.5522 Y-.714
N200 X-.6141 Y-.739
N210 X-.721 Y-.7711
N220 X-.8483 Y-.7994
N230 X-.9858 Y-.8203
N240 X-1.1225 Y-.8316
N250 X-1.2523 Y-.8327
N260 X-1.373 Y-.8239
N270 X-1.4846 Y-.8056
N280 X-1.5878 Y-.778
N290 X-1.6833 Y-.7415
N300 X-1.7675 Y-.6984
N310 X-1.7996 Y-.6792
N320 X-1.8798 Y-.6245
N330 X-1.9616 Y-.5565
N340 X-2.0022 Y-.5169
N350 X-2.0368 Y-.4787
N360 X-2.0701 Y-.4362
N370 X-2.1113 Y-.3706
N380 X-2.1362 Y-.3182
N390 X-2.1637 Y-.2333
N400 X-2.1772 Y-.1407
N410 X-2.1764 Y-.0472

[Joesph Jackman]

to post the mcx file change the extension to something like .zip. then mention that those who download your file need to change .zip to .mcx there maybe another way that i don't know to upload files here but this will work.

[Superman]

Here is a snippet of the code. It is a 3d solid model imported as an ipt file from inventor. And yes the rounded shape was originally a spline. ANy help would be appreciated. I cant figure out how to post the mcx file.
N160 X-.2462 Y-.6215
N170 X-.3587 Y-.6508
N180 X-.4993 Y-.6954
N190 X-.5522 Y-.714
N200 X-.6141 Y-.739
N210 X-.721 Y-.7711
N220 X-.8483 Y-.7994

This is point to point code. There are a couple of conditions that force out this type of code
1/- toolpaths obtained from splines will force out point to point code
2/- "Filter" or "Tolerance" settings are turned OFF
3/- arcs are disabled on that particular plane

the size of the facet is contolled by the filter settings, larger number = large facet = shorter length of code = less accurate toolpath

for filter and tolerance settings, they must be enabled either within your post and/or in the control file ( under "Arcs" )

to change a spline into an arc, use the edit/simplify ( you may have to break the spline into shorter lengths to have success --- ie a "C" may simplify into 1 arc but a "U" would need breaking up )

[mattfurches]

I am creating toolpaths from a 3d solid model that i imported from inventor. Can I simplify/edit the model edges that were created in inventor using a spline in mastercam? Looking at the model i have selected the simplify command and chosen the splines but i dont see that it has selected or highlighted anything on the model. Im wondering if you have to simplify the spline when it is first drawn in 2d?

[mattfurches]

To clarify, i created the part in inventor. The rounded edge was created using a spline in inventor. Now that I have imported the solid into mastercam how do i change that solid edge into an arc when it was created using a spline?

[WallyL7]

I noticed your other post about learning the software. I'd also suggest you learn a little g-code - which is the reason I wanted you to post your code. If you knew a little about code you would have seen it was all lines and not arcs.

It seems you are putting the cart before the horse.

[mattfurches]

While I am certainly not an expert in any of this I do recognize the code as lines not arcs. My question was more directed at why I was getting that code instead of Arc code. If I wasnt clear I apologise.

[WallyL7]

No problem. Your first question was "When the mill is making a 2d curve, just a simple arc, the face looks like a series of short lines."

which leads us to believe that the mill is programed to cut an ARC and not just a series of lines...lol.

[cadcam]

We call this faciting and this most like coming from a Spline curve. what are you picking as an edge wire from the solid or the solid?
This why it helps to see the file to see what you are picking and what type of path. are you trying rotat this on the 4th at the same time. there are allot of factors missing here.