Sharp cornered mdf doors

[GlenP]

Hey all, anyone out there with a PRS standard cutting mdf doors with a vbit to create sharp outside corners? I have having alot of trouble getting the cut clean as right now the cutter will take too much out of the corner and leave a awful profile which will require tons of sanding to clean up.

[Gary Campbell]

Glen...
Are you talking about sharp outside corners on interior carving, or on the outside profile?

Here is a set of vanity doors we do for a local designer that has a recessed beaded wainscot design. A V bit is used on the outside corner of the "panel" to get the required square corner. Also required was that the beads line up between the door and draw fronts above.
Heres the set:


3697

Closup of the corner:


3698
Gary

[GlenP]

Hey Gary, I am talking about the sharp corners on the interior panel corners. I am doing some sample doors and using aspire. For some testing I just made a simple rectangle and did a profile cut to cut on the inside with sharp corners turned on. Every test cut the cutter makes a corner that looks like the cutter diameter is incorrect but I have changed the cutter diameter values both up and down with no success in corner. I never have much luck posting pics here from our camera but I can send you the pics of the cut to your email if required. I have done lots of mdf doors with the rounded corners but want to do the sharp panel corners and have also been asked about doors just as you have created.

[Gary Campbell]

Glen...
To make the border,like you I drew and selected a rectangle, selected inside profile, 90 degree V bit, .25 depth and sharp inside and outside corners using VCPro5. It sounds as tho you did exactly the same, so I am a little stumped.

You can send the pics if you want, and I will look them over and post so that those wiser then I may be able to get you in the right direction.
Gary

[GlenP]

Thanks Gary. I will send them in the morning to you. I am hoping someone with a PRS Standard will chime in as that is the machine I am using. I do not use vacuum for hold down just screws to the spoilboard. I was using a 120 degree 2" diameter cutter with even a low .125" max cut depth to rule out too much down pressure and the material rising while the corner is being cut. I have tested close to both x rails to check for x motor backlash and the same cut. Heck I tested in the middle of the bed and same cut. When you look at the cut it just looks like the cutter is going too high (deep)into the corners when going up to create the sharp corner. I was wondering if IU reduce the cornering values to see if it is just backlash on the standard motors. ????? Thanks in advance for any help and ideas.

[myxpykalix]

GlenP go to www.xat.com (http://www.xat.com) and download
"jpegoptimizer". It will allow you to keep your pictures at 640x480 but shrink the kilobyte size to under 50k so you can post your pictures here.

3699

Gary- on your wainscoting to my eyes it looks like the beading is inset (i know its all one piece) and is lower than the surface of the rails and stiles or is it all the same height?
Nice looking though.

[GlenP]

Hey guys, here is the post on the vectric site to see a pic.
http://www.vectric.com/forum/viewtopic.php?f=3&t=6415

[Gary Campbell]

Jack...
Yes the interior panel was pocketed out .125 before the beads were cut into it. This is a 4 bit job

1/2" downspiral pocket out panel .125 (from surface)
90 Vbit IS profile .25 deep around border
1/8 pointed roundover .21 deep (includes .125 from pocket)
3/8 compression to cut profile climb/conv

Heres the Setup in VCPro:

3700

And the preview:

3701
Gary

[tkovacs]

Glen,
I have a PRS standard and have never seen anything like what you are posting on the vectric site.
Looks to me like when the corner is cut the z axis is not moving up fast enough to keep pace with the xy motion.

Terry

[zeykr]

I think as someone else has mentioned, that the actual bit angle or size is different from the settings in the tool database. It's not at all unusual for v bit to be off several degrees or for endmills to be a little under or over the stated size.

[myxpykalix]

I went and looked at the picture you reference and my feeling is that if your tooling was bad you would have problems thruoghtout the whole cutting and not just in the corners.
Have you checked your drawings carefully to make sure you don't have any duplicate vectors in that corner causing you this problem?

[myxpykalix]

gary...i wasn't sure my eyes weren't playing tricks on me. That detail gives the part a nice shadow line and gives it the appearance of being rail and stile constructed. Cool

[Gary Campbell]

Glen...
I looked over on the Vectric forum at this also. Dont have any magic, but it appears to lean more towards a mechanical than software issue. Have you checked the Z pinion, bearings and motor to rack for proper adjustment?

Gary

[Gary Campbell]

Jack...
Even tho they are time consuming to cut, we get paid well for them. We got the job because the MDF & TFoil door companies can't, don't or won't give all 3 specs: square corner, line up beads on 3 door set and round beads like wainscot of old. Glad I don't have to sand & finish them.

Gary

[myxpykalix]

Gary
see arrows...your sides are thicker then your bottom/top which looks good but I wondered if there was some rules of thumb you go by to decide the differences? what are your sizes here? (if you know)..

3702
To my eyes because this design is taller than wide this difference looks good however if the design was more equally square my sense is that it would look better if both the top and side were of equal thickness right?

[Gary Campbell]

Jack...
Usually I would say yes. This job had a LOT (40+) drawer fronts. The designer used 2.5" for the style(side)width and 1.5" for the top & bottom rail height so that the many banks of drawers looked better. This was also applied to the door fronts. I needed a consistant width for the styles that was an increment (double) of the spacing on the beads. I couldnt say it was wrong.
Gary

[GlenP]

Gary, I have checked and done a maintenance on my pinions and they are fine. No play in pinions. A guy had posted similar issue with a buddy and I think Robert Ball (aka batman) got his fixed and tweaked to work somewhat better. The only thing that makes me scratch my head about only a mechanical issue is all four corners look like this and it is consistent anywhere on the table and every time. If only a mechanical thing I would think I should see some variables in corners or cutting somewhere. ??? I have a order for some doors and if I can't pin point this and correct I may have to outsource to meet timeline. I did notice when I was a Lowes the other night that a white vanity had a similar but not as noticeable mark in the corner of the doors. Jack if my tooling angle is off it will look like the picture when vcarving as the software uses the diameter of the cutter for the depth of vcut for the sides and bottom and use the angle to calculate the cornering distance. I have checked my bit and it is 119.5 degrees but when I change the angle values to that it makes no significant increase in cut quality. Still would involve ALOT of sanding. Terry how are your PRS motors? Are they quiet and zippy sounding or do they sometimes make a rattle sound (hard to describe)?

[Gary Campbell]

Glen...
I have chased down similar problems in the past. It is very difficult, if not impossible, to tell if there is play without a solidly mounted dial indicator. Sometimes mounted in the spindle over a metal plate. Sometimes magnet'ed to the plate checking side play in both the X and Y direction. In each case, Z extrusion bearing, pinion to rack or eccentric adjustment was the culprit.

If you problem lies in the Z, and I assume it does, it will be consistant over the full range of the table. You could also have a "rocking horse" condition where one of your X car (gantry) wheels is higher (off the rail) than the other 3. this would also cause your condition as the weight from the spindle transferson direction change or Z plunge.

I would check the Z with the dial indicator both directions against a 1/2" drill rod in the collet. Then if you have a full collet set, as I do, chuck it in the collet. Once the dial indicator is in place place very firm (30-40#) pressure in every direction, dont forget up and down. Check with spindle close and far from the table. Make sure that the Z extrusion V rollers are consistant thruout the complete range of movement. IF they become loose at some point it is a problem. It is good to take the motor off and move the Z thru full motion by hand to get a feel.

Dont forget, you will most likely never feel or see a movement that makes the divot in your pictures. Good Luck!
Gary

[cnc_works]

In looking at the photos on the Aspire site, I remembered a post on a very similar problem earlier. Thread url: http://www.talkshopbot.com/forum/messages/33572/38348.html. It didn't look as if a real solution was ever found or at least posted.

Sorry I couldn't contribute more, but maybe this will save some troubleshooting time.

Donn

[rb99]

Can you repeat the problem with a different square?

How about trying a triangle shaped tool path instead of a square? Then you could rotate it and see if it is only when the forces are from a certain angle?

Also if Gary has no problem with his file maybe he will send you a file to cut that he knows works and perhaps he could cut yours?

RIB

[GlenP]

I am going to try some other shapes and also some letters later today. I have done alot of vcarve cutout letters for customers and they seemed to be fine. The file I was trying to test cut was only a simple rectangle with a profile cut with sharp corners turned on. One thing I did notice with sharp corners turned on as it creates a parameter for the tooling automatically and I can edit this parameter. Have to look and see how that number is represented. I am going to make it my mission to get this corrected.

[jerry_stanek]

Have you tried cutting on the line? I just ran a test cutting inside and it didn't cut the starting corner right but when I cut on the line it cut fine.

[dmidkiff]

Glen,
You might try using a 90 degree V-bit to get the result you are looking for. Hope it works.
Dave

[tkovacs]

Glen,
I have on rare occasion heard a rattle sound and have always took it to mean that I was pushing the machine too fast and slowed down the feed rate. I typically run xy between 2-4 ips and z 0.5-1 ips but I recently did a 2 hr cut on some foam at 6 ips xy 2 ips z and all went well.

A question - does the outside corner of the V cut lie at the intersection of the extended straight side edges? If it does I would think that would eliminate tooling issues.

Terry

[rb99]

I think it is a software bug...


RIB

[tmerrill]

Richard,

If the preview mode isn't showing a problem, than I very much doubt it's a software bug. I've also used a test file with the ShopBot previewer which inputs the generated toolpath and it doesn't show any problems.

Another consideration is there are a lot of us cutting similar designs frequently and to my knowledge only Glen and one other person have reported an issue like this.

Tim

[GlenP]

Hey guys glad to have the feedback. I am not sure about a software thing as Gary is getting very nice results but also he is using vcarve 5.0 and I am using aspire. I know say deal just more bells and whistles but???? Also Gary is running a alpha (nice one I might add) with a spindle and I am on a standard with a router. Starting to think and as Gary points out that a combination of minor things are combining to give this result. A bad router bearing itself may be doing this??? I am tight for time at lunch but I am going to try some other testing tonight and also post my file for all to see. Yak at ya later guys and thanks.
GLen

[tmerrill]

Glen,

You can always verify this with an email to Vectric support, but the functions in Aspire and VCP that are the same share the same exact code. Aspire just has the additional 3D features. So there should be no issues because Gary has VCP and you have Aspire.

Tim

[Gary Campbell]

Glen...
Tim is right. I dont use have Aspire, but the postP would be exactly the same. I highly doubt this is a difference between VCPro & Aspire.

Can you select all your vactors for one door and email me an (ACAD)DXF? I will toolpath with VCPro and send SBP back to you. This may prevent you from following a possible wrong path.
Gary