Feature request

[Forrest Chapman]

Thermwood,

I wonder if anyone else would like to be able to set cut direction to each bit instead of for all bits. And also for all your skinned parts the option to skin going one way and cut thru going another.

When useing a 3/8\" comp bit and cutting conv. the bit will flex into the part. So when the cleanup pass comes around since it doesn't have the same force applied it will leave a small lip at the bottom edge. When cutting climb cut the bit will flex out and when it cuts thru on the second pass it will flex less cleaning up the part and leaving no lip.

Some material is okay to cut climb like mdf, but plywood and melamine in order to get really clean cuts require conv. cut and that is where the problems may arise. Mostly the long narrow parts are areas where the router ramps to full speed and the bit will flex the most.

The ideal situation is to climb cut on the first pass and conv. cut on thru cut on plywood. I could skin all my parts and run at 1200 ipm and not have to worry about any movement or left over ledges.

If you guys want to talk directly call me at 864-226-5256

Forrest

[Brian Shannon]

That makes pretty good sense Forrest. I'd like to see that feature.


Brian

[Joe Soto]

I vote for that Forrest.
Joe

[Mark Hesketh]

this might actually be what is happening to alot of our parts. we are having issues where on any part that gets a skin pass, a small ledge is left on the part all the way around. it is most noticable on mdf parts. the ledge that gets left is only about 1/64-1/32, but it is quite visible depending on the material, and really upsets everyone else down the line. is there any way that we can aviod this issue?

[Forrest Chapman]

Guys,

For mdf its quite simple. Just cut in climb direction. The edge quality is the same but the line will dissapear. This is something we have struggled with for the 4 years we've had our router. Now I'm sorry I didn't say something sooner.

I did think of one possible fix for plywood. The outside edge is okay with climb cut especially when it cuts twice. Its not perfect but okay. The dados however are no good with climb cut. No matter how good your tooling is the dados will be fuzzed out the wahzoo. If you cut alot of plywood you can set up your dado tooling with a reverse spindle and it will cut opposite of your outline bit. This will require an opposite hand bit as well.

Forrest

[Mark Taylor]

Forrest...how fast are you running your 3/8 bit in plywood and/or mdf? Are you actually pushing 1200 ipm? That's twice as fast as they recommended when we were trained up in Dale.

Mark

[Rob Frenette]

Count me in on that one Forrest. Painfull having to sand that little lip off before edgebanding small melamine parts. 1200 IPM sounds a little fast for a 3/8 cutter. We use a 1/2\" compresion at 700 IPM and we still get the lip.

[Forrest Chapman]

Guys,

You would actually be surprised at how well plywood cuts at this speed. 18000rpm and 1200ipm conv. cut. The cut is clean and there is almost no dust left on the table. We also cut 5/8 melamine this fast but found that the edge would not band well because of the bit flexing. Long runs like an end panel is where it showed up the most. Since you cannot run melamine in climb cut the only way I know to avoid this line is to do a rough cut maybe 2k bigger and then clean up on the cut thru.

We are currently cutting 3/4 and less plywood with a 3/8\" 2flute comp. 18000rpm and 850 ipm climb on most everything. We cannot run faster or we would but in climb mode we lose edge quality.

We are currently cutting 3/4\" mel. same bit same rpm but 700 ipm. 5/8 mel is same bit same rpm but 800 ipm. both in conv. cut.

We are currently cutting 3/4\" and less mdf same bit same rpm at 850 ipm in climb mode. This is fine and exceptable.


I hope Thermwood is listening. This is something that all machine owners that I know go through regardless of make or software.

Forrest

[Ryan Hochgesang]

Thanks everyone for your input on this topic. I will certainly submit this request to the Software Engineering Dept. here at Thermwood and I'm sure it will be given a great deal of consideration.

[Forrest Chapman]

Thanks Ryan for responding,

Mark, when we got our router they set us up with a 1/2\" 2 flute running at 18000rpm and 400ipm so a lot has changed. I would say that 600ipm is a safe all around speed but your bit life will be shorter unless your running 15000 rpm or so. I cannot cut 3/4 mdf at more than about 1000ipm with my 10hp motor. Once the rpms start to drop it deteriorates till the bit breaks.

Ryan, I would love to talk about this in more detail if you need you've got my numbers.

Forrest

[Bill Rutherford]

Count me in.

Actually I just logged onto the forum to post a similar request. Our idea was to be able to specify cut direction for a certain material group but being able to specify direction for each tool within a group would be even more valuble.

The reason I finally am getting around to posting this today is as follows:

Last night we tested some interpolated holes in plywood. Because we had been running melamine all day the machine was set to climb cut, neither my operator or I picked up on this. We got the hole sized out perfectly. This morning we loaded the plywood, changed cut direction to convetional (our standard for plywood) and cut the first sheet not stopping to think about the already tested holes. Thankfully we tested the dowel in one of the holes on the first sheet (and not the tenth) because the conventional cut was giving us a much cleaner hole that was now to sloppy.

With Forest's idea we would have been able to set the tooling in the group with the melamine for climb and the tooling in the group for the plywood for conventional and I would be happy then I am now!!

Thanks.

[Forrest Chapman]

Bill,

Thats exactly the idea. Another place is with dovetail dwrs. If you run your 1/4\" bit in climb for the tails it will flex slightly out making a tapered edge which fits tight on the outside edge and more loose on the inside edge. Its like a wedge. But running the dovetail bit and outline cutter in conv. give a much cleaner surface.

Forrest

[Joe Elbert]

Good idea Forrest count me in.

Joe

[David Hall]

Just another thought on the subject, that might be a little easier to implement.

If the first pass of a double pass cut were performed outside the part perimeter by a user defined amount. (say .030\") and the second pass was performed on the line. This should eliminate the \"lip\" when double passing on a conventional cut.

Although a little clunky, this could be implemented as a \"first pass outline tool\" and \"second pass outline tool\" selection. The first pass tool could be a virtual tool pointing to the same physical tool as the second pass tool. By setting the first pass tool diameter .060\" larger than the actual tool diameter, it would cut outside the part perimeter by .030\". When combined with a little behind the scenes \"additional part clearance\" we could elminate the problem for conventional cutting.

If implemented this way, I expect I might actually use two different tools for some solid stock applications.


Regards,
Dave

[Mark Hesketh]

this is more or less the way that Panelmetrix handles this problem. It runs the first pass something like 0.010\" larger than the outline, then does the clean-up pass right to the outline. Seems to work great on the doors I cut. Shouldn't be too hard to implement (this coming from a non-programmer)... could even give it a toggle switch in the settings so that you can choose whether you want to utilize it or not.