adjusting arc smoothness

[Marshal]

Is there a way to adjust the smoothness of an arc in MCam X4? I know in SolidWorks, it's pretty much just adjusting the image quality. So I've adjusted the quality in SW, and it's nice and smooth there, but when I bring it into MCam, it's still not smooth, but a series of lines.

 

This seems to translate to the mill (POS Hurco VM1), which then makes round objects look less round.

 

Thanks in advance for the help

[Guest]

yeah, edit >> simplify

 

Turn your splines in arcs instead

[Marshal]

quote:

---

yeah, edit >> simplify

 

Turn your splines in arcs instead

---

The problem is that I'm brining most of the models in from SW, and they aren't splines, they're arcs to begin with.

 

I guess, come to think of it, the surface is what's choppy, the circle I used to make the toolpath isn't choppy..so I'll revise my question:

 

Is there a way to make it so the mill actually follows that stupid circle exactly, instead of creating a bunch of facets on the part? Basically, I think there needs to be more points in the code, or it needs to use an actual arc path instead of moving linearly from x1 to x2

[dolphin1]

yes you need to seperate the surfaces from the wire path on different levels. then just pick the arc from the wirepath.

[Marshal]

quote:

---

yes you need to seperate the surfaces from the wire path on different levels. then just pick the arc from the wirepath.

---

I've done that. In fact, I'm not using the surface/wirepath at all. I've created new geometry (a circle) in MCam to use as the toolpath, and it looks round in MCam, but doesn't come out smooth on the mill. This leads me to believe there's a setting somewhere to make it go around a circle instead of doing segments (which gives the faceted look).

 

I know there's a g-code for doing a circular path, but why isn't MCam doing that automatically when cutting out a circle?

[Guest]

What's your code look like?

 

You getting R's or IJK values?

 

BTW, visually, if your arc "looks" jagged in MCAM but IS a circle, then the visual quality has zero affect on the gcode generated.

[Marshal]

quote:

---

What's your code look like?

 

You getting R's or IJK values?

---

Nope, just x's and y's. That's the reason I'm thinking there's a setting somewhere that's goofed up. Shouldn't it be doing a G02 or G03 instead of a G01?

 

The situation is that I'm trying to cut around the outside of a 0.575" cylinder with a 0.125" endmill. Should work just fine, and would if it'd do a circular path instead of linear

[Guest]

open up your control def, go to the arcs branch and see if support arcs in XY is checked? If not check mark it.

[CJep]

Marshal,

If you are using a contour toolpath try enabling the Arc Filter / Tolerance. Set the filter ratio to 1:1 to start, activate create arcs in XY then set the min and max arc radius

[Marshal]

quote:

---

open up your control def, go to the arcs branch and see if support arcs in XY is checked? If not check mark it.

---

It's checked. Should the "allow 360 arcs" be checked as well? That's something that our main machinist has wondered about, because he said he's always had to break an arc into two pieces.

 

quote:

---

If you are using a contour toolpath try enabling the Arc Filter / Tolerance. Set the filter ratio to 1:1 to start, activate create arcs in XY then set the min and max arc radius

---

I'll look into that, thanks

[Guest]

How about a z2g file?

 

Something isn't "quite" right here, on a circle with a contour you should be getting arcs, period, no filter needed.

[CJep]

Marshal,

If you need to break the arcs at the control in MDI before you run the code, I would suggest that you set the arc breaks in the control def file to break at 180. Use the drop down to the right of arc break options.

 

Also a good way to make default changes to the control def is to open it through the machine def in the settings drop down. This way as you green check your way out to accept the changes you will be prompted to replace the machine def in the existing part file. If you go directly into the control def you will need to do a machine def replace in the machine group properties to affect the changes in the existing part file.

[Marshal]

quote:

---

If you need to break the arcs at the control in MDI before you run the code, I would suggest that you set the arc breaks in the control def file to break at 180. Use the drop down to the right of arc break options.

---

I don't want to break the arcs if the machine would do a full circle (which I don't think it will). So right now that setting is probably fine.

 

Perhaps that's the overall problem, that the circle hasn't been broken? Maybe I need to break that circle into 180 arcs and then it'll do the circular toolpath

[Guest]

get me a z2g and I remove ALL of the questions and tell you exactly what's happening.

[CJep]

typically if you're getting linear code instead of circular interpolation it has more to do with geometry, however you mentioned earlier that you had created an arc and used that for the toolpath geometry if all the settings in the control def are correct, there could be a setting in the post that is forcing linear output

 

a zip to go file is the only way find out what is going on, have you contacted tech support through your reseller?

[Marshal]

and what exactly is a z2g?

[jeff]

zip 2 go file.

 

Just a thought,Do you have linerize (sp?) helixes checked?

That would force a G01 instead of G02-G03

[CJep]

go to the help drop down the toolbars, under the help drop down you will find the Zip to Go utility, click on the utility to launch it, make certain that the check boxes for mill, post processors and toolpath are checked then click on the button in the lower left to create the zip to go file, a zip file will be created in the documents area of your computer with the file name and the file extention .z2g, all the selected files associated with your part file will be in the zip file

[Eric Witthus Prototek Engineering]

Marshal,

Where is your arc located? When generating the code Mastercam checks the rounded endpoints to the calculated endpoints and if the difference is greater then the value set in the tolerance it will linearize the arc.

[Marshal]

unfortunately, I'm either an idiot (entirely possible), or am just unlucky (just as possible). I can't log onto the FTP server to put the file up...what a wonderfully lucky and productive day I'm having today

[Marshal]

Eric, the center of the arc is at the origin, and it's 0.575" in diameter.

 

We've had this trouble with the facets since before I started here, and it almost seems random, so I'd like to understand why it does that, and how to fix it

[Guest]

you can email to me and I'll put it up

 

jmparis65 at gmail.com

[Marshal]

sent

[Guest]

I asked if you have splines

 

and to use edit simplify

 

[Guest]

File sent back with a circle.

 

Analyze Properties, then edit simplify will work wonders with arcs

 

code:

---

N100 G20

N102 G0 G17 G40 G49 G80 G90

( CUT AROUND CYLINDER TO -0.150 )

N104 T3 M6

N106 G0 G90 G54 X.3502 Y0. S4278 M3

N108 G43 H3 Z.25

N110 Z.1

N112 G1 Z-.01 F10.

N114 G2 I-.3502 J0.

N116 G1 Z-.02

N118 G2 I-.3502 J0.

N120 G1 Z-.03

N122 G2 I-.3502 J0.

N124 G1 Z-.04

N126 G2 I-.3502 J0.

N128 G1 Z-.05

N130 G2 I-.3502 J0.

N132 G1 Z-.06

N134 G2 I-.3502 J0.

N136 G1 Z-.07

N138 G2 I-.3502 J0.

N140 G1 Z-.08

N142 G2 I-.3502 J0.

N144 G1 Z-.09

N146 G2 I-.3502 J0.

N148 G1 Z-.1

N150 G2 I-.3502 J0.

N152 G1 Z-.11

N154 G2 I-.3502 J0.

N156 G1 Z-.12

N158 G2 I-.3502 J0.

N160 G1 Z-.13

N162 G2 I-.3502 J0.

N164 G1 Z-.14

N166 G2 I-.3502 J0.

N168 G1 Z-.15

N170 G2 I-.3502 J0.

N172 G1 Z-.05

N174 G0 Z.25

N176 M5

N178 G91 G28 Z0.

N180 G28 X0. Y0.

N182 M30

%

---