Inlay - male part has 'ridges' I don't see in the preview

[309cnc]

Hi again eveyyone,

I am working on a VCarve inlay and am getting pretty good results except for a few little ridges in the male part I can't figure out.

I followed the steps in the various tutorial videos out there pretty much step by step and the process seems to working very well (once I had the vectors all figured out....).

Cutting the female went without a hitch and came out very clean. The male however shows some ridges / artifacts I don't understand. They are not present in the preview and cutting the file several times always led to the exact same problems.



The picture only shows one of them but I have about 5 of them in total. I am gluing them together now and so I don't have a picture of the final inlay yet but I am pretty sure this will show up as a small step in an otherwise very smooth curve.

I have cut with different feed speeds down to 30 ipm and that does not seem to make a difference. Recalculating the tool path does not seem to make a difference in the preview or the actual cutting path. I left the board in place and recalculated and ran with a slightly lower starting depth. Same result just a little deeper....

Hmm.....

Anyone have a guess as to:

- operator error somehow
- VCarve 9 issue,
- Postprocessor issue
- other?

Thanks.....

[garylyb]

It's probably in the font.

The font you are using probably has a bunch of points there. Look at it in the vector view, you should be able to see it there.

You need to edit it or use a different font.

[309cnc]

Ok, good point. I did not explain what the design is or how I arrived at it....

Initially, I only had a jpg. The specific font used in the logo was not available to me. So I let VCarve convert the bitmap to a vectors and looked at it. It had lots points on the curves and I was not happy with it.

So I decided to start over and re-created the entire image by tracing each letter and line with the various design tools available in VCarve. Mostly lines and ovals that I 'massaged' using the node mode and Bezier curve handles. I then joined, cleaned up and grouped vectors as needed. As far as I can tell, the result were single clean curves.

Here is a partial screen shot from the (single) curve in question:

[garylyb]

What does it look like using the node edit tool?

That picture can hide a lot of stuff in the vectors.

[309cnc]

Is this what you are asking about?

[garylyb]

That's what I wanted to see, but it's very clean, and shouldn't cause that problem.

I've seen fonts that create a ton of nodes when converted, but that one looks good.

You can try tweaking the curves a bit, but I don't see anything that would cause that problem.

Is it always the same letter? If it cuts that letter the same way in different sizes in different parts of the table, then it's probably not hardware, but in the software somewhere.

[309cnc]

Thanks garylyb

It happens on different areas of the design. Here is another example. Both 'o's are affected in the same bottom left area.



Same in the vector node view:

[garylyb]

Is that where the bit enters and exits the path?

That's where the green square is.

[stevem]

What speed are you cutting at? It may just be to fast!

[garylyb]

If that's where the bit enters and exits, then there is something that is probably loose.

Turn off the machine, and try turning the x,y,z axis by hand, there should be almost no play.

[309cnc]

stevem: last run was at 30 ipm

garylyb:

- The green square is about at the top (12 o'clock) for both vectors
- Did not watch it at that particular time. I may try cutting again this weekend and waiting to catch those specific areas....
- No play that I can tell

[Deleted]

Your source vectors have minimal control points so they aren't the problem. It could have to do with having too much backlash but it would be easier to tell with your G-code file uploaded. Sometimes even with the best source vectors, there are issues created because the bit is too large to get in the fine details where letters are too close (adjust for larger kerning) and there are many small moves to get the bit in the confined space. The other thing may be because the line is at your start point, adding lead in / lead out may help. It's always better to diagnose a problem by uploading files as we are just guessing without them. Your CRV file is best but sometimes a G-code file will work as we can load it in a simulator and check it out.

[traindriver]

If you upload the .crv, I'll give it a try on my AR8 and see if I get the same result.

[309cnc]

Thank you @fean and traindriver. I'll try to get to the shop later today and get the file(s).

I spent most of yesterday changing lots of settings trying to see if anything made a difference. Probably did another 10+ cuts..... Here are some findings (or lack of):

- The ridges are repeatable precisely.
- That flipped capital 'C' came out with that ridge/tab at that 8pm position no matter what I changed: Feed rate (down to 10 ipm), plunge speed, cutting depth, you name it....

- In an attempt to reduce cutting time I isolated the 'C' vector and cut it: No more ridge! What I mean by isolated is I removed everything from the original file except that one vector and cut it only.....



- I added the next vector ('o') to the left of the 'C' back into the file and the ridge on the 'C' came back! No ridge on the 'o'. Seems the proximity of the two curves has something to do with it.... So I added the third vector back in (another 'o') and sure enough.... now there is a ridge on the 'C' as well as the first of the two 'o's. Not on the third though....

 

- I added a ramp: This removed the ridge but created other (small) cutting errors in other places around the 'C'.... So adding ramp(s) changes things as well...

Stay tuned for the files.....

Thanks

 

[garylyb]

Well, this is getting interesting.

The error is either in generating the g code, or the hhc when it converts it to machine movement. You have a new machine, and probably a new hhc, min is the original hhc.

When you post the code, I'll try it here also. Post both the crv and the gcode file.

Best regards,

Gary

[Deleted]

Would it hurt the design to adjust the kerning to add more space between the characters so the toolpath part of the CAM can do a better job and not introduce non-existent errors? The Vectric toolpath software, even for Aspire, is very primitive and can get confused easily and make mistakes so sometimes you have to change your design to get help the software along. Fusion 360 doesn't have these problems as it's much more advanced CAM.

[309cnc]

Here we go..... (finally)... I had to start over because with all the iterations I tried I got lost in too many files and probably delieted a few I didn't intend to... ;-)

Anyway, attached are pictures of the latest run and I point out 4 areas of concern. I am also including the .CRV files and the .MMG file.

VCarve calculates a Pocket tool path with an end mill as well to clear out wider areas. But I am not cutting that file and so I am not including it. Only the tool path cut with the V-bit.



Details:




Yep, reached the limit for # of attachments.... Files in the next post.....

[309cnc]

the files.....

Cookery test file.crv (932 KB)

Cookery test file_Summary.html (120.62 KB)

VCarve1.mmg (171.21 KB)

[309cnc]

Just in case I have not mentioned this before: I never had an issue cutting the female board. Nice smooth cuts all the way around. The male inlay is where the problems occur....

[stevem]

Just wondering if you have tried asking the same question on the Vectric forum. Those guys are very helpful.

[309cnc]

Feb 12, 2018 11:22:43 GMT -5 @fean said:

Would it hurt the design to adjust the kerning to add more space between the characters so the toolpath part of the CAM can do a better job and not introduce non-existent errors? The Vectric toolpath software, even for Aspire, is very primitive and can get confused easily and make mistakes so sometimes you have to change your design to get help the software along. Fusion 360 doesn't have these problems as it's much more advanced CAM.

I don't want to change the design of the logo. But.... maybe one workaround could be to cut each inlay vector by itself. I would then have to glue each one into the female part separately but it could be done, I suppose....

[309cnc]

Feb 12, 2018 17:10:37 GMT -5 stevem said:

Just wondering if you have tried asking the same question on the Vectric forum. Those guys are very helpful.

Had not thought about that yet. Being a newbie I did not really know if this would likely be an Axiom problem or not. Now that most of you are pointing me in the direction of VCarve..... that is probably a next step I should take....

[Deleted]

Thanks for the files, if you look at the toolpaths, your problem occurs where the clearance "triangles" meet up with the long sweep of the curves. The short answer is that the toolpaths are good but your tool model doesn't exactly match your actual tool geometry. The V-bit tool model doesn't include a flat area at the tip so the geometry is off slightly which is causing your problem. Below I have the tools for the Amana 45700 as a V-bit and as an engraving tool, the latter allows you to put in the correct geometry which will render in Vectric what will actually happen when you carve with that tool and allow for corrections in your situation. Personally, I prefer the Amana RC-1075 and its inserts for just this reason, it has finer tips available and more accurate geometry in addition to lower cost of replacements.

Attachments:

vbit.tool (919 B)

actual.tool (842 B)

[309cnc]

@fean: Thank you for looking into the file.

Some of this is new to me but I think I am getting what you are telling me:

Below is what you refer to by saying: "where the clearance "triangles" meet up with the long sweep of the curves".




I loaded the 'actual.tool' model and in there I see the option to set the flat tip width. I calculated a couple tool path and noticed how changing this width affects the path generated:



This is something I obviously can not do with the standard V-Bit model and you say making use of this feature could resolve my problem. Correct?

So here is the plan: I will leave my current V-bit cutter in place, but use a new tool path created with the 'actual.tool' model and then start cutting, correct? If needed, I can 'play around' with the width of the flat and make more cuts....

Appreciate your help!

PS: I will look into the Amana tool you mentioned.

[Deleted]

Yes, I think you're getting it. When you touch off the tool, because it doesn't come to a real point, where the taper is actually located is different by the width of the actual tip flat spot. It doesn't matter as much where there is airspace around your desired result, your surfaces will just be located off slightly from where they should be but where things come together you get things like what you have. What bit are you using for your V-carving? Another trick I sometimes use instead of V-carving is to use the V-bit for a profile as you have more control over actual placement, but at the same time, it's more work than letting the software figure things out, right or wrong. As for the Amana tool and inserts, there is a 1/2" shank version available that takes the same inserts.

[309cnc]

Valentine's day caused an interruption in my troubleshooting.....  Hope to get back on it over the weekend.....

[309cnc]

I am using a Bosch Vbit cutter: www.boschtools.com/us/en/boschtools-ocs/carbide-tipped-v-groove-bits-85219m-27105-p/

Cutting right now using the flat tip model.... I will post the results.

[309cnc]

Bummer.....

looks like I have several more ridges now than I did before..... This first pic shows the result of having the width of the flat tip set to .03"



Ran it again changing the width to .06" and .01". Hmmm.....

[309cnc]

Ran the file again cutting into insul board (the pink foam sheets) and the ridges were much less pronounced. Hmm....

So I started wondering if maybe my Bosch PR20 router has so much radial play that every time it plunges down onto an already angled surface it also moves sideways. So I changed it out to the DeWalt DW611 router and ran it again. The ridges were all back.....

Pretty frustrated right now..... Spent upwards of 20h troubleshooting and trying different things but don't seem to be any closer to a solution than when I started....

Any chance someone can run it on their machine and see what happens? It is about 12"w x 6"tall. The 90deg V-bit cuts around 1/2" deep so a 3/4 board would work.

As suggested, I will try to figure out how to ask these questions on the Vectric forum as well. I say trying because I don't want to have to type everything again.... Anyone done this before? Can I perhaps just link on that board to this thread here?

Any other suggestions welcome.....

[traindriver]

Hmmmmm . . . . the plot thickens . . .  I don't know how to break this to you, but I'm afraid I have bad news.  I cut your file on my machine and it appears that you may have a case of mouthus angularous, or, in the south Georgia vernacular - you ain't holding your mouth right because I didn't have the issues you're having.





I used your file with only two changes that should have no effect on the problem whatsoever:  I changed the Z Zero Position to the top surface, and the XY Datum Position to the lower left, since that's the way I usually set my jobs up.  I cut it out of a piece of scrap cherry that was held down with clamps, using an Amana 90 degree V-bit (part #45712)  I actually prefer to use 60 degree bits and occasionally a 30 degree bit, depending on how thin the details are - the walls are steeper and you leave more stock so it's less likely to tear out.  I took the part off the machine and took the picture before removing any of the fuzzies left over so you could see the unadulterated version.  This is the setup of my v bit.


My machine is an AR8 Pro with a water-cooled spindle and I just upgraded to Vectric VCarve Pro version 9.010.  I can't think of anything else to add, but if you have any questions, let me know.  If it's any solace, there appears to be nothing wrong with your file.  At the plant I used to work at, when things like this happened I chalked them up to either solar flares, or the unproven fact that the plant was built over an ancient Indian burial ground.