Surface High Speed "Core Roughing" Lead off of Material?

[neurosis]

I have a part that I am trying to rough out using this function. I cant seem to get the tool path to lead in off of the material. It seems to only want to ramp in to the top of the material along the profile or helical in to the top of the material. Is there any way to force this path to lead in off of the material rather than ramping in to it?

 

I should add that this part seems a perfect candidate for surface rough contour, I was just wondering how to get the surface high speed paths to work on this particular part. I have to guess here, but I think that the issue is the tool diameter being larger than the distance from the surfaces to the edge of the stock.

 

I can post a picture of that part and stock if necessary.

 

[ 08-11-2010, 08:38 AM: Message edited by: Neurosis ]

[Mike-T]

I often have to modify my stock boundry to get what I want.

[nhraguy]

Maybe use "area clearance" instead of "core roughing". Area clearance will start off of part.

[Colin Gilchrist]

You've got it backwards. Core roughing is supposed to work from the outside in. Area Clearance is supposed to work Inside out.

[nhraguy]

It figures, I don't use those toolpaths that often but thought that it was the other way around. My bad.

[neurosis]

The only way that I have been able to get the path to lead in off of the material was to modify my stock boundary to way oversize. This created extra passes and huge lead-ins. Very inefficient tool path. I am still trying to get this to work!

[RandleXX]

I think it is under Linking Parameters-Leads-Linear entry/exit ?

[Colin Gilchrist]

Send it in to QC...

[neurosis]

Colin,

 

I may send it in and see what they say. I am using the path in what may not seem to be what it was intended for although I "think" that it is. I will try to post a picture monday before wasting anyone's time in the qc department.

[Kendo]

anybody ever get the surface high-speed toolpaths to quit using helical or ramp entry into "open" pockets where the tool could just feed down off the material?

[neurosis]

anybody ever get the surface high-speed toolpaths to quit using helical or ramp entry into "open" pockets where the tool could just feed down off the material?

 

 

There are allot of cases where the tool ramps in to material in a very inefficient way. I have mostly learned to ignore it. We are working on a part right now using opti-rest where the final depth only needs to cut .1 in to the material at the bottom of the part. Rather than just ramping down in to the .1 of material, it ramps from the previous depth. That is 1.15 deep that it is ramping in to air.

 

It has been quite some time since I made this post and I rarely use core roughing anymore but I remember the situation. When ever I would use a tool that the diameter was over %50 more than the distance of the surface to the edge of the part it would force the tool to ramp down on to the material. I do not remember which part this was to see if that is still the case.

 

I have also had problems with the opti-paths where if your arc radius was larger than the distance of your material to the edge of your stock, it would just leave those areas uncut. I think that has been fixed? I havent noticed that issue since using X6. I remember one of the parts that I had an issue with this on and could check this one out.

[?Mark]

" I cant seem to get the tool path to lead in off of the material."

 

Set tool containment to "outside" and check "add offset distance to tool radius". That way your containment boundary needs to match the outside shape of material being cut and no need to further mess with it.

I do it all the time and it works great.

In x6 and not looking back

[neurosis]

" I cant seem to get the tool path to lead in off of the material."

 

Set tool containment to "outside" and check "add offset distance to tool radius". That way your containment boundary needs to match the outside shape of material being cut and no need to further mess with it.

I do it all the time and it works great.

In x6 and not looking back

 

 

Mark,

 

when you do this, do you leave the offset distance at the default (1/2 of your tool diameter)? Or do you set it to 0. (minus half your tool diameter in the field)?

 

 

I just ran an optirough operation in a part that was known to be an issue in the past. Nothing has changed. If you set your (in x5, tool path radius in X6, MIN toolpath radius) to greater than the distance from the edge of your material to your part, it will not cut that area at all. It completely misses it. The attached picture shows the area (ignore the top of the part) that was left uncut.

 

If I set my containment boundary to outside and check "add offset to tool radius" since my tool diameter is 1" and my step over is only .1, it makes four full revolutions around the outside of the part before it even starts to cut material.

 

Why do I use a .5 (or larger) arc radius you ask? Because at 1000ipm, a large radius is much smoother of a transition than a .1 radius.

[?Mark]

I almost always keep the "Total offset distance" at 1/2 of tool diameter (default).

 

" it makes four full revolutions around the outside of the part before it even starts to cut material." <<<< four???

It makes one full revolution here, which in most cases works good (at least for me) as an extra precaution since most of my stock material is slightly over sized and it ensures a smooth initial tool engagement, which at speeds I'm running at is critical...

[neurosis]

Like I said, my tool diameter is 1" so 1/2 of the tool diameter is .5 (not trying to give a math lesson). Since you are essentially telling the system that your stock boundary is, .5 in this case, LARGER than it really is, and because of the strategy that I am using to remove the material, it cuts allot of air. My step overs are .1 .5 /.1, well... I think you get it. The cutter makes four full revolutions before it cuts.

 

What I ended up having to do in this case was extend the ends of the material rather than the whole boundary in order to get it to clean the ends up. I could have also just created a separate operation to clean up the ends.

 

I guess my point is, why is this necessary?

[?Mark]

Got you... my engagement is 45%, hence 1 pass around only...

[Brando]

neurosis, are you willing to email me the file,, i use this path all the time and i could probably help

[neurosis]

I cant email you the file but it is easy to reproduce.

 

All that you have to do is use any surface or solid part, create a stock boundary, set your toolpath radius to a size greater than the distance of your material/stock boundary edge of your part and generate the path. It does this in both core roughing and opti.

 

I use these paths for just about everything that we do here. If you notice, I posted the original topic in August of 2010. I have found several work arounds to these issues since. I just wanted to check today to see if some of them had been addressed. And they have not.