Surface contour

[So not a Guru]

It's been awhile since I've needed to use this path for undercutting, and I can't figure out why I can't get it to make the undercuts. Can someone take a look and see if I'm missing something obvious?

test.mcam

[Colin Gilchrist]

 

See if that helps...

[scottvan]

I got it to work better by using the top surface as drive, instead of check.

[nickbe10]

Had a quick look in 2019. WCS came in not normal to the top surface, so your tool is shanking out.

3 drive surfaces selected but I could only see a single surface, you might want to try a more restrictive containment.

Maybe some of this was caused by import into 2019 without proper migration?

[So not a Guru]

I got it working with flowline. Actually, I had it working the 1st time I did it with flowline, but I thought it was wrong from looking at verify. Apparently verify thinks my lollypop is a ball. 

[billb]

On the third tab page of the Finish/Contour operation's parameter dialog, check that you have enabled the (new) "Detect undercut" checkbox. 

[So not a Guru]

50 minutes ago, billb said:

On the third tab page of the Finish/Contour operation's parameter dialog, check that you have enabled the (new) "Detect undercut" checkbox. 

I tried it both ways, it doesn't get the full undercut either way. The way I read the help file seemed to say that it must be unchecked to cut undercuts. I could be reading it wrong. In any case, for this my preference was flowline & it works well.

[So not a Guru]

Just now, So not a Guru said:

flowline & it works well

I did have to use a different tool however.

[billb]

Oh, the help probably mentions unchecking the "gap gouge check" checkboxes (short and long) on the Gap Settings dialog.  That is still true - you want to disable gouge-checking of the keep down motion when undercutting (if it sees a gouge, it will "lift" the tool - not what is wanted here).  I'll reread the help to see if there is anything that should be updated.

Glad you got what you needed.

[So not a Guru]

14 hours ago, billb said:

Oh, the help

This is why I'm not sure if it's supposed to be checke or unchecked, in order to allow undercuts. It states that it is enabled when an undercut tool is selected, but (if checked?) disables undercutting.

[billb]

You're right - that 2018 help is a bit terse (and confusing).  It looks like it was revised for the 2019 help:

Detect undercuts - "Only available when an undercut tool is selected.  When selected, undercutting is enabled."

That is better but I'll ask around and see if we can do more.

[motor-vater]

I too am very frustrated with this path right now I got 3 days into a project that requires many undercuts because of inside cavities and a lip around the opening. Not only do I never get to a good toolpath but it takes like 20 minutes to generate every time I make a change... errrrr. Trying out multi axis options like triangle and parallel with no luck either. thought I had it today when I discovered the multi-axis paths have like 2 or 3 places to pick your planes. This is on a horizontal so once I figured that out thought it would be ez mony, but no I am still up the creek, I feel like if I get the planes figured out I will make the constant z parallel work, but apparently its beyond my scope of understanding.... Why is it so hard to use undercuts!!!!!!

EDIT. The undercuts selection box completly takes out the toolpath in multiaxis, probably because I am forcing it to 3 axis and select undercuts only has 3+2 or 5 axis options.... So frustrated right now...

[Matthew Hajicek - Singularity]

If it's taking 20 minutes per try you might do what i was doing back in the 90's on a 266MHz Pentium.  Do a sample path with much looser tolerance and stepover, and play around until it looks right, then tighten the tolerance and stepover and regen.

[Manofwar]

17 hours ago, motor-vater said:

I too am very frustrated with this path right now I got 3 days into a project that requires many undercuts because of inside cavities and a lip around the opening. Not only do I never get to a good toolpath but it takes like 20 minutes to generate every time I make a change... errrrr. Trying out multi axis options like triangle and parallel with no luck either. thought I had it today when I discovered the multi-axis paths have like 2 or 3 places to pick your planes. This is on a horizontal so once I figured that out thought it would be ez mony, but no I am still up the creek, I feel like if I get the planes figured out I will make the constant z parallel work, but apparently its beyond my scope of understanding.... Why is it so hard to use undercuts!!!!!!

EDIT. The undercuts selection box completly takes out the toolpath in multiaxis, probably because I am forcing it to 3 axis and select undercuts only has 3+2 or 5 axis options.... So frustrated right now...

Motor-Vater. The easiest way to use a very specific plane that I have found in the multi-axis paths is to use conical limits. Draw a line of the z axis direction of the plane you want. Turn on limits under tool axis control. In the dialog for limits turn on conical and limit the angle to the defined line. Then if you want 3 axis, type in 0 in both fields. If you want movement give it the limits you want to use.

[scottm085]

 

If your using multi-axis make sure the box "Extends tool to infinity" is unchecked it you want to do undercuts.

[Teh Bear without Brains kinda idiot]

I got it to work better by using the top surface as drive, instead of check.

 

~~~~~~~~~~~~

I make undercut milling on  the daily basis.

Never use check only drive surfaces.

Saves me a lot of pain

HTH

 

 

[Colin Gilchrist]

On 10/4/2018 at 8:54 PM, motor-vater said:

I too am very frustrated with this path right now I got 3 days into a project that requires many undercuts because of inside cavities and a lip around the opening. Not only do I never get to a good toolpath but it takes like 20 minutes to generate every time I make a change... errrrr. Trying out multi axis options like triangle and parallel with no luck either. thought I had it today when I discovered the multi-axis paths have like 2 or 3 places to pick your planes. This is on a horizontal so once I figured that out thought it would be ez mony, but no I am still up the creek, I feel like if I get the planes figured out I will make the constant z parallel work, but apparently its beyond my scope of understanding.... Why is it so hard to use undercuts!!!!!!

EDIT. The undercuts selection box completly takes out the toolpath in multiaxis, probably because I am forcing it to 3 axis and select undercuts only has 3+2 or 5 axis options.... So frustrated right now...

What kind of tool are you using? Is it a lollipop or a slot mill? Sometimes instead of a full radius slot mill, I'll define the tool as a slot mill with a corner radius, and make the radius .0001 smaller than nominal. This gives a .0002 "flat", but it really won't matter much in terms of the tool motion that is generated. It seems to help with getting a clean path, and also speeding up the calculation time.

[jlw™]

I would use flowline on both surfaces.  Your lollipop will not clear the full undercut either.

 

Check out the motion in the attached file.

test.mcam

[So not a Guru]

41 minutes ago, jlw™ said:

I would use flowline on both surfaces.  Your lollipop will not clear the full undercut either.

 

Check out the motion in the attached file.

test.mcam

Yes, I ended up using a 300° lollypop instead.

[motor-vater]

Thanks for the heads up guys, the tool extends to infinity helped but I am still not there. I will mess with some of the things Colin recommended when I am back on that job. Thanks as always