v-inlay technique problems
v-inlay technique problems
Hi everyone,
While I have had decent success with V Carve's built-in inlay toolpaths, I also need to use the v-inlay technique for finer details that require sharp corners. And I'm having a problem. For the most part the male pieces are coming out well and "fit" ok in the female pockets. But as you can see in this close up, something is off. I am not getting sharp corners, and it's almost like the v bit is slightly dogboning the corners. The straight portions machined quite well and are a good fit for the male parts.
I am using a 60 degree v bit for both cuts. Female pocket machined to .15" flat depth using the v-carve toolpath with a 2% stepover to clear out the pocket. Male parts are mirrored, offset outwards .18" and then v-carved at .1 start depth and .1 flat depth to create inverse parts.
Any ideas?
Thanks!
Brian
While I have had decent success with V Carve's built-in inlay toolpaths, I also need to use the v-inlay technique for finer details that require sharp corners. And I'm having a problem. For the most part the male pieces are coming out well and "fit" ok in the female pockets. But as you can see in this close up, something is off. I am not getting sharp corners, and it's almost like the v bit is slightly dogboning the corners. The straight portions machined quite well and are a good fit for the male parts.
I am using a 60 degree v bit for both cuts. Female pocket machined to .15" flat depth using the v-carve toolpath with a 2% stepover to clear out the pocket. Male parts are mirrored, offset outwards .18" and then v-carved at .1 start depth and .1 flat depth to create inverse parts.
Any ideas?
Thanks!
Brian
-
- Vectric Wizard
- Posts: 517
- Joined: Sun Apr 30, 2006 10:04 pm
- Model of CNC Machine: shopbot PRT Alpha 96x48
- Location: New Hampshire, USA
- Contact:
Re: v-inlay technique problems
Your bit may be "a bit off" in terms of angle. Check this http://forum.vectric.com/viewtopic.php?f=3&t=2164.
Paul Z
Paul Z
Re: v-inlay technique problems
Thanks Paul Z. That is intriguing and, well, I never would have thought about it!Paul Z wrote:Your bit may be "a bit off" in terms of angle. Check this http://forum.vectric.com/viewtopic.php?f=3&t=2164.
Paul Z
I read through that thread, and near the end someone's post got me thinking. In addition to bit angle discrepancies, could my problem also be stock that isn't flat enough or z zero that is slightly off? I suspect those "dogbones" in the corners happen either when the bit plunges or retracts. If zero is off or stock isn't flat, the bit could end up plunging too early, right, which would cause that extra little bite out of the corner?
If so, I guess I have to investigate both issues.
-
- Vectric Wizard
- Posts: 447
- Joined: Thu Oct 02, 2014 1:49 pm
- Model of CNC Machine: FMT Patriot 4 x8
Re: v-inlay technique problems
Have a look at the bit's tip is there a flat? I think there is a greater likelihood of having a flat tip or dull tip than a cnc ground cutter being out of specified angle. The effect of a flat tip that isn't specified in tool geometry is similar to one with a wrong angle. The cure is to draw the tool with the flat as a form tool or engraving bit.
I don't see much evidence of not flat workpiece.
I don't see much evidence of not flat workpiece.
- FixitMike
- Vectric Wizard
- Posts: 2173
- Joined: Sun Apr 17, 2011 5:21 am
- Model of CNC Machine: Shark Pro Plus (retired)
- Location: Burien, WA USA
Re: v-inlay technique problems
Why are the male parts offset outwards? I can see that that is not the cause of the problem you are asking about, but I am curious why there is an offset outwards. I've not done any offsetting and the results have been fine.
bk3132 wrote: Male parts are mirrored, offset outwards .18" and then v-carved at .1 start depth and .1 flat depth to create inverse parts.
Thanks!
Brian
Good judgement comes from experience.
Experience comes from bad judgement.
Experience comes from bad judgement.
Re: v-inlay technique problems
Mike, I offset the vectors so that I can make the software carve the male part inverted as pictured. Is there another way? I'd love to know! Thanks.FixitMike wrote:Why are the male parts offset outwards? I can see that that is not the cause of the problem you are asking about, but I am curious why there is an offset outwards. I've not done any offsetting and the results have been fine.
Re: v-inlay technique problems
That's interesting. I will have to take a look tomorrow. It's the Onsrud 37-82 60 degree V bit, which, I believe, isn't supposed to have a flat tip. But then again I might have given it one! To tell you the truth, I have always worried about that particular bit and the automatic z zero plate/zeroing process. I have to believe that dulls the tip over time, right??tomgardiner wrote:Have a look at the bit's tip is there a flat? I think there is a greater likelihood of having a flat tip or dull tip than a cnc ground cutter being out of specified angle. The effect of a flat tip that isn't specified in tool geometry is similar to one with a wrong angle. The cure is to draw the tool with the flat as a form tool or engraving bit.
I don't see much evidence of not flat workpiece.
- FixitMike
- Vectric Wizard
- Posts: 2173
- Joined: Sun Apr 17, 2011 5:21 am
- Model of CNC Machine: Shark Pro Plus (retired)
- Location: Burien, WA USA
Re: v-inlay technique problems
I draw a rectangle (or other closed vector) around all of the male parts and select it as well as the parts for the VCarve toolpath. I use a flat area clearance tool to clean up the wide areas. That way I have only a single piece to glue in place. (Unless, of course, it turns out to be more convenient to cut the male part into separate pieces for the glue up.)bk3132 wrote:
Mike, I offset the vectors so that I can make the software carve the male part inverted as pictured. Is there another way? I'd love to know! Thanks.
Good judgement comes from experience.
Experience comes from bad judgement.
Experience comes from bad judgement.
-
- Vectric Apprentice
- Posts: 86
- Joined: Wed Feb 15, 2017 2:03 pm
- Model of CNC Machine: 2 SCM Routech Record 120s(1999, 2001)
Re: v-inlay technique problems
This is your problem.bk3132 wrote:
Mike, I offset the vectors so that I can make the software carve the male part inverted as pictured. Is there another way? I'd love to know! Thanks.
Watch the toutorial again, you are missing a huge step. You need to copy the artwork, mirror it, draw a bounding box and then vcarve the whole thing inside the bounding box to get the mirror image male plug
Re: v-inlay technique problems
It’s not the problem. The male inlay parts are fine. What I’m doing is essentially what you have written. In this case, though, it’s easier to glue up the inlay parts individually. So my bounding boxes are simple offset vectors, and all told I machine far less this way and can arrange the individual male parts for optimal stock usage rather than as they would actually inlay on the piece.potzmannwoodshop wrote:
This is your problem.
Watch the toutorial again, you are missing a huge step. You need to copy the artwork, mirror it, draw a bounding box and then vcarve the whole thing inside the bounding box to get the mirror image male plug
-
- Vectric Craftsman
- Posts: 142
- Joined: Tue Jan 24, 2006 11:57 am
- Model of CNC Machine: ShopBot PRS Alpha
- Location: Imperial, PA USA
Re: v-inlay technique problems
Brian,
A long time ago my Shopbot was VCarving with the same type of results. Turns out that the Z axis pinion was not seated on the stepper shaft far enough and was binding. When you get to corners in the geometry the Z pulls up while still moving in the X and Y. If it doesn't retract high enough you get what appears to be an overcut in those areas.
Check the integrity of your Z axis and make sure that everything is ship shape.
Bill
A long time ago my Shopbot was VCarving with the same type of results. Turns out that the Z axis pinion was not seated on the stepper shaft far enough and was binding. When you get to corners in the geometry the Z pulls up while still moving in the X and Y. If it doesn't retract high enough you get what appears to be an overcut in those areas.
Check the integrity of your Z axis and make sure that everything is ship shape.
Bill
Re: v-inlay technique problems
Well, I think I have my answer. After tugging on the machine every which way I can't say I feel much of any slop. So I cut a bunch of squares defining the 60 degree bit's geometry differently for each of them, and they ALL had the same extra scooping out at the corners. So I looked at the bit more carefully and see now that it's probably rounding at the tip. Then I ran the original v inlay pocket toolpath using a newer 90 degree v bit, and presto, sharp corners.
Is it possible that my z zero plate is contributing to the dulling/rouding of v bits?? I cringe every time I watch that point hit the metal plate...
Thanks everyone.
Brian
Is it possible that my z zero plate is contributing to the dulling/rouding of v bits?? I cringe every time I watch that point hit the metal plate...
Thanks everyone.
Brian
-
- Vectric Craftsman
- Posts: 142
- Joined: Tue Jan 24, 2006 11:57 am
- Model of CNC Machine: ShopBot PRS Alpha
- Location: Imperial, PA USA
Re: v-inlay technique problems
Brian
I don't think that's the case. The bit I used for this has been in service for over 2 years.
Bill
I don't think that's the case. The bit I used for this has been in service for over 2 years.
Bill