How can I keep this Surface Finish path on the outside?

[Mic6]

How do keep this finish path to do the outside only? What you see is contour. Flowline is giving me the same trouble. My drive surface is the OD face

 

 

[MotorCityMinion]

Cap the part.

 

 

 

 

 

[MotorCityMinion]

Double post.

[BernieT]

In Ver 9.1, I would use the green geometry as a 'boundry' - set for 'outside'. I think.........

 

 

Should be the same in ver X+

 

 

You may have to play with the inside/outside/offsets

 

 

HTH

[Mic6]

I filled holes top and bottom, but the path wont follow the angle of the surface.

 

[MotorCityMinion]

The part appears to have an inward draft. I don't know how successful the boundary would be. Is your tool defined as being able to under cut for that distance? Got enough radial clearance as in a loli pop tool or key seat cutter and so on?

[Mic6]

The part appears to have an inward draft. I don't know how successful the boundary would be. Is your tool defined as being able to under cut for that distance? Radial clearance?

 

That it does. I want to cut this surface in this operation, otherwise I can't hold it in the next op. My tool is a full radius keyseat cutter with plenty of clearance. With flowline, the preview lines follow the angle, but when it's done processing, it only cuts at Z0.

[gcode]

flowline should do this if you turn off gouge checking

[MotorCityMinion]

sf contour, gouge checking disabled.

undercut (Small).bmp

[Colin Gilchrist]

I just did a Contour Toolpath successfully on a surface like yours. It follows the angle of the undercut. I used a Slot Mill (.25 thick) and set it to a Corner Radius of .125.

 

Is your surface normal pointing outwards? In 'Gap Settings' you can try turning off the gouge checking for transition and retract. Also, in 'Advanced Settings' try changing the rolling motion to "over all edges".

 

Flowline will also get you what you want.

 

With the Undercut, you'll need to use "Direction" for the Lead In/Out, or use the Arc/Line entry options.

 

Flowline will also work for this, but you'll have to disable the gouge checking there as well.

 

Edit: Beat by MCM...

[Mic6]

Gcode: I keep gettign errors when I try to turn gouge-check off

 

MCM: Did you use check or containment?

 

Time to go home, 14hrs is enough. I'll revisit this at 5 tomorrow. Thx guys

[MotorCityMinion]

Check. How the @#!$ do I upload a pic without it being an attachment or link to a hosting site.?

[ajmer]

make sure that the containment boundary is not stoping it from cutting the surface, try removing the containment and regening it

also you have to cap the surface and select it as either drive or check

[Hardmill]

make sure that the containment boundary is not stoping it from cutting the surface, try removing the containment and regening it

also you have to cap the surface and select it as either drive or check

 

 

^^^^^^^ +1

 

If you select it as drive just set your min -z- jus below the top.

Dont always have to use as check surf, it sometimes nets better results.

 

 

 

 

 

 

 

 

 

 

 

 

 

 

PEACE

[Mic6]

Man, this is still making me nuts. So I selected the OD angled surface as drive in surface finish>contour. Clicked the top cap as check. Cut Depths minimum Z-.005, surface normals to the outside, gouge cjecks are off and I still get the same toolpath that feeds at the same diameter all the way down. (post #5)

 

No containment is used

 

What other parameters did you use in that pic MCM?

[Hardmill]

Man, this is still making me nuts. So I selected the OD angled surface as drive in surface finish>contour. Clicked the top cap as check. Cut Depths minimum Z-.005, surface normals to the outside, gouge cjecks are off and I still get the same toolpath that feeds at the same diameter all the way down. (post #5)

 

No containment is used

 

What other parameters did you use in that pic MCM?

 

send it ill take a look hardmill(at)gmail(dot)com

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

PEACE

[?Mark]

Looks like the tool is defined as custom. Redefine it as slot mill with 2 equal radiuses (for full radius) or a lollipop. MC is extremly picky for undercuts...

[Hardmill]

Mail, and yeah i did ditch the custom tool.

 

 

 

 

 

 

 

 

 

 

 

 

 

 

PEACE

[Mic6]

MC is extremly picky for undercuts...

 

Now I know! Thanks everybody. I've been doing the :old forumheadslam: for the past 4 hours!

[?Mark]

cheers to hardmill for nailing it

[Mic6]

cheers to hardmill for nailing it

 

. ..said the timestamp

[Mic6]

ALMOST there! What in the world are all these dumb jumps everywhere? My min depth is Z-.075

 

 

 

EDIT: nevermind. Thanks again everybody. Finally get outof this dang chair and cut something!

[?Mark]

Hard to avoid if top edge is not at the same z. Lower your starting z to just below top edge (relative to center of tool radius) and adjust gap settings to larger number (1 inch ?)

[Colin Gilchrist]

To eliminate those jumping motions, try increasing your Gap Size. Set the radio button to "Distance" and enter a value. My typical Gap Setting .25 inches. This will tend to keep the tool in contact with the surfaces. Sometimes I'll go back into the Parameters and increase this to 1-2" if I'm still getting retract motion where I don't want it.

 

Make sure you look at the exit motion of the tool. When doing an undercut, the default tool motion at the end of the path is a vertical retract. This can cause your tool to gouge into the part you just cut. There are two things you can enable to stop this. You can use the Entry/Exit Arc/Line options, or you can use the "Direction" button to give your tool a lead in/out vector.

 

Also, to eliminate the little transition steps between the cuts, you can enable the "spiral limit" function. This will cause the toolpath to move down in a constant spiral motion, but will also dramatically increase the size of your NC code.

[MotorCityMinion]

Sorry I didn't get back with you sooner, f-in comp issues. Everybody else has stated it already though. The part I used was 10' in dia. I set my gap to 10." Care full, big gap settings can cause issues that don't jump at at you untill it's too late, study the tool path in back plot and verify as this technique does not care about tangency or plowing through adjacent surfaces. Verify and check for gouges if your not sure. Start Z- based on half the tool +.001. Not a custom tool either. I defined it as a slot mill with .124 corner rads, .25 wide.

 

Off topic some here, but setting a negative Z, that is to say below the top of your surface, (could very well be a positive number as well), for your start point, and using larger gap settings works well with quite a few different scenarios, not just undercuts or negative draft or contour tool paths.

 

My preference when I want a pristine path is to extend the surfaces up above the part by a distance greater than the tool rad, then set Z values with depth cuts, this way, the tool will start at Z0.00 and not turn that first cut into a Screaming Demon. I often model parts with the intent that I'm going to machine it and could use the extra meat in the model just for this purpose, so I'll create 2 models, structuring the build of the actual part so that the machining model is easy to create. I'll do some surface offsets and extends while I'm in SW at the same time for machining purposes.