2D contour collision

[Anonymous]

I can't figure this out. This is a simple 2D contour cut, cutting out 8 holes. Each of the holes is the same dimension of 0.2" and the operation is using a 0.1875" end mill. For some reason it doesn't include one of the 8 holes giving an error of:

Warning: A contour was not machined because the given lead parameters would cause a collision!

Generation completed with 1 warning(s) in 828.0ms.

What is causing this collision? I'm using:

HSMWorks 2016 R4.41148
SolidWorks 2016 x64 SP3.0

I've attached some screenshots, notice the upper-middle-right hole is missing a toolpath.

[ivan.stanojevic]

Did you try to lower down a little bit your lead in/out parameters on the linking tab?

[Anonymous]

The lead-in and lead-out are both turned off. I haven't tried changing the numbers before turning it off. Is that what you mean?

[Anonymous]

I just realized i left out the last screenshot. Notice the Lead in and Lead out are both unchecked.

[ivan.stanojevic]

It is hard to say without the actual part..

[ivan.stanojevic]

Ok, I recreated your part and I had the same issue..

But when I clicked on entry position and chose some of the holes as entry position it worked.

But it is strange though.

I have attached the part. Maybe somebody from the support team should check this issue.

[Anonymous]

OOOH! The entry position seems to solve it.

I've honestly never used the entry position before. I just let HSM decide.

I just attached my part. I've made some minor changes to the file, but if you look Job (1) - 2D Contour2, you'll quickly see the error. If I select any position it does seem to go away.

Thank you Ivan!!

[ivan.stanojevic]

You welcome 🙂

[Anonymous]

Darn it. This solution worked for my last part, but the attached part has an entry position but still has a collision. I've tried different combinations of entry positions and it still doesn't include all 4 holes.

[Steinwerks]

So I have to ask, why use such a close tool for that hole? You're asking an end mill (or a machine for that matter) to interpolate a .0094" diameter. That's not exactly ideal. Why not use a 1/8" and helix bore?

[Anonymous]

Well this is crazy.

I just tried clicking on random spots for the entry position... If I click on the vertex corner where "Coordinate System 1" is, it works. If I choose one of the circles, it doesn't work. If I leave the entry position out, which is the default, it doesn't work.

[Anonymous]

Because 1/8" bits break on me all the time. I've had terrible luck with boring hole operations. 3/16" upcut, 2 flute carbide bits with contour cuts have worked great for me for most 2.5D operations. It's my goto operation in HSM.

I've also tried just drilling with jobber bits with exact dimensions and they produce awful, unclean holes in aluminum. Probably because the jobber bits I got are just crappy. But also because it seems to plunge too fast with a drilling operation. This is all on a Shopbot desktop mill.

[Anonymous]

Although I did just start using 1 flute 1/8" bits last week and I haven't broken any yet. Maybe I'll experiment again with helix boring operations. In the past, the boring operations seem to push too hard for my 1/8" bits. Could just be an incorrect speed/feed setting. That is certainly an area of milling that I've never felt extremely confident in.

[Steinwerks]

My suggestion for a starting point with a 1/8" 3-flute carbide end mill is spin it as fast as your spindle goes, helix at 2-3° with a maximum stepdown of 1/2 diameter (.0625 in this case of course) and about .001/flute feed. Some kind of chip evacuation is highly recommended. I avoid 2-flutes personally, and never plunge into the material (it works, but hard on the tool).

[kb9ydn]

---

@Anonymous wrote:

Because 1/8" bits break on me all the time. I've had terrible luck with boring hole operations. 3/16" upcut, 2 flute carbide bits with contour cuts have worked great for me for most 2.5D operations. It's my goto operation in HSM.

I've also tried just drilling with jobber bits with exact dimensions and they produce awful, unclean holes in aluminum. Probably because the jobber bits I got are just crappy. But also because it seems to plunge too fast with a drilling operation. This is all on a Shopbot desktop mill.

---

Do yourself a favor and get a set of screw machine length drill bits.  They're shorter and therefore much more rigid so they don't walk. For really small holes you should also spot drill first.  Trying to interpolate holes that small is honestly a waste of time and small endmills.  Plunging speed shouldn't be an issue if you can feed Z slow enough to interpolate.

C|

[ivan.stanojevic]

---

@Steinwerks wrote:
So I have to ask, why use such a close tool for that hole? You're asking an end mill (or a machine for that matter) to interpolate a .0094" diameter. That's not exactly ideal. Why not use a 1/8" and helix bore?

---

I was thinking about asking him the same question.